PDA

View Full Version : Questions on using a moving gantry style mini-mill...



Davek0974
14-03-2016, 03:09 PM
Getting near the end of my router/mini-mill build now and need to start looking at how to run jobs, i have a couple lined up already;)

I'm not new to milling - been running a Bridgeport for some years now, not new to CNC - been using a plasma table for a year now, so that should all help. I use SheetCam to produce my G-Code and I think I have it pretty much sussed for the mill now, just looking for tips.

This is the first job - pretty complex but what better way to learn;)
17925
It's from 5mm 6061 Aluminium, has plenty of 3mm holes, slots, square features, its about 320mm long.

So far I am looking at using a 2mm carbide 2-flute cutter, mist coolant, I have figured out how to get sharp corners, also how to spiral-down to cut the holes.

Questions -

1 - I have used a calculator for feeds and got 24,000rpm, 487mm/min feed, 1mm DOC, these seem reasonable?

2 - I am unsure of DOC - this is input rather than output on the feed calculator - how do you know how much bite to take at one pass?

3 - Holding tabs to keep it together on the outside cuts, I'm guessing three or four, 0.5mm thick or less?

4 - Use the one cutter and go straight to dimension or split and do a roughing & finish passes?

5 - Use a bigger cutter for the roughing outside then switch to the 2mm for the finish?

6 - Features like the oval hole - leave it to fall out or use tabs again?

Any suggestions appreciated, I realise this is fairly adventurous but I would like to get these made in-house to increase my profit margin considerably ;)

Thanks

Clive S
14-03-2016, 04:55 PM
How are you going to do the 90' corners?

Davek0974
14-03-2016, 06:18 PM
How are you going to do the 90' corners?

There is a tool-path option in SheetCam that runs the cutter diagonally into the corner just enough to allow the resulting corner to accept a square cut object - a neat feature and with a 2mm cutter its barely noticeable.

routercnc
14-03-2016, 08:32 PM
Hi Dave,

Taking each point in turn:

#1 Only ever used a 3mm carbide, nothing smaller. I think it would snap on my machine at those rates but possibly depends on how rigid your machine is.

#2 DOC for 3mm carbide has been about 0.3mm for me. It's quite possible I'm shortening it's life doing this but it works well but I only use it occasionally and it's still going strong.

#3 I'd use 4 holding tabs. Now in Vectric Cut2D the thickness is relative to the bottom of the cut. For that cut I would ask for 6mm total depth to make sure it went right through. Therefore 0.5mm tab would not actually hold the part and I'd need to input a tab depth of 1.5mm to get 0.5mm. I think I'd go for at least 2mm tab to make sure it did not vibrate on the last finish pass.

#4 If the part is complex (long run time, chance of an e-stop or other problem) then I'd do a roughing cut leaving 0.1mm for the outside as a finish cut.

#5 I would not attempt all that with 2mm cutter! Use 6mm or 8mm if possible to cut most of it out, then finish pass with the same bit, then go in again with the 2mm for the detail.

#6 Don't leave the oval hole as a free cut. When the cutter gets to the end the oval part will jam against the bit and mark the work, then fly across the workshop. AMHIK.
You can use tabs, but it is a pain to clean up by hand inside there, so better still is "pocket" it out (turn it all to swarf).

As a strategy I think I would:
Spot all the holes (leave finishing for the drill press)
Pocket out all the internal holes and slots (i.e. not an internal profile)
Rough profile the exterior with 6 or 8mm carbide, leaving 0.1mm
Finish profile the exterior with 6 or 8mm carbide in one full depth pass (but still use same tabs as when roughing)
Switch to 2mm cutter and profile the outside again to get the detail then profile the inside of the pockets
Cut away the tabs and tidy up the edges by hand

Davek0974
14-03-2016, 09:36 PM
As a strategy I think I would:
Spot all the holes (leave finishing for the drill press)
Pocket out all the internal holes and slots (i.e. not an internal profile)
Rough profile the exterior with 6 or 8mm carbide, leaving 0.1mm
Finish profile the exterior with 6 or 8mm carbide in one full depth pass (but still use same tabs as when roughing)
Switch to 2mm cutter and profile the outside again to get the detail then profile the inside of the pockets
Cut away the tabs and tidy up the edges by hand

Thanks for that, interesting stuff, my response...

I really don't want to drill the final holes, IMHO, spiralling down should work ok, will need to test it.

Pocketing out the waste - brilliant point, probably never have thought of that one;)

Rough profile exterior - makes sense but favour a 6mm rather than going bigger.

Finish profile exterior with big cutter - if its only got 0.1mm to go, I'm not sure of the point, a 2mm solid carbide should handle that in one pass AFIK - test again.

The smaller internal shape/pocket would need a smaller roughing cutter, probably 4mm, why not go to finish on the same tool?

Tabs are the same in Sheetcam, bottom upwards. So if i have an aluminium bed, I would not want to request a 6mm cut on a 5mm sheet, I was thinking of using a sheet of stiff card or some-such between, I use a lot of 0.4mm hard card at work and that would likely work well, cut would then go to work plus 0.2mm.

I'm generally against babying cutters, on the Bridgeport I find they are happier when taking a proper cut, within the abilities of the machine, but not tickling the metal, especially with carbide which has a larger edge radius than HSS and needs to 'cut' the metal.

Some good points though, noted, thanks

JAZZCNC
14-03-2016, 11:14 PM
#1 With cutters less than 3mm I work on 30% diameter DOC.

#3 Wouldn't use tabs I'd use Onion Skin of 0.1mm. This gets rid of any chance of bed damage and removes risk of lifting.

#4 Rough and Finish passes. I'd use Large tool for Pocketing and Roughing then use small tool for Finish pass and corners cleanup etc.

Davek0974
15-03-2016, 07:27 AM
Thanks Jazz, more good tips.

0.6mm DOC on a 2mm cutter sounds reasonable.

I had seen onion skinning used on the woodworking forums but how do you go about cleaning it off on a job like this or is it easier than i think?

Rough and finish - large and small makes sense, would use the same process for shapes like the large oval or just use the large tool staring to finish?

Thanks

JAZZCNC
15-03-2016, 02:32 PM
I had seen onion skinning used on the woodworking forums but how do you go about cleaning it off on a job like this or is it easier than i think?

The part breaks out easy. Often it breaks out clean but even if the 0.1 skin is left on in places it just snaps off clean. Then quick whip round edge with De-bur tool and done.


Rough and finish - large and small makes sense, would use the same process for shapes like the large oval or just use the large tool staring to finish?

Depends on Job really. If could get away with using same tool then I would but if Got to use small tool then it pays to use large tool to hog away material quickly then finish with small tool at full depth.
Often people try to avoid tool change and use same small tool but this fasle economy in several ways.?
Large tool will do it in fraction of time and with much less wear which more than offsets the tool change time. The small amount of material left also means the smaller tool is much less likely to break and also wear is less.

All it means is you have to think a little differently when you Cam the part and order the toolpaths are generated when large amount of tools are used.
Instead of having a operation which roughs then finishes in same toolpath before going to next area meaning lots tool changes. ie: Pocket operation then profile operation.
Instead you just have each operation do the roughing with large tool then create a separate set of operations for the finish passes with small tool.
This way when post processed all the Roughing passes are done before the Finish passes so only one tool change for all operations.

Hope that makes sense.?

Davek0974
15-03-2016, 02:41 PM
Thanks JAZZ,

I was unsure if the onion skin would be enough to hold the part for the finish op's, have been messing in sheet cam and running simulations etc, seem to have it sorted i think but i can now re-order the processes to do all the roughing first.

What sort (if any) lube/coolant do you use on aluminium? I have enough parts in now to build a pressurised fog-less system but just wondering what people put in them :)

Back to the CAM, shapes like the odd shaped internal part on my drawing, I have roughed out the bulk with a 5mm tool, that leaves of course 2.5mm rads in all the corners, are you saying to finish cut that with the 2mm tool in one pass?

Do lead-ins and outs feature or forget them for the minute?

JAZZCNC
15-03-2016, 03:05 PM
What sort (if any) lube/coolant do you use on aluminium? I have enough parts in now to build a pressurised fog-less system but just wondering what people put in them :)

I use WD40 type lube but oil/parafin mix will work.


Back to the CAM, shapes like the odd shaped internal part on my drawing, I have roughed out the bulk with a 5mm tool, that leaves of course 2.5mm rads in all the corners, are you saying to finish cut that with the 2mm tool in one pass?

Yes will be ok in this case because your now side cutting and the tiny amount left won't hurt anything. However it's not recommended to use same size tool as the radius. ie: 2mm Rad use use 1.9mm or smaller Dia tool. This means the tool won't be cutting on two sides in the corner so won't chatter or snag and break the tool. Which can happen on really small tools. Larger tools just usually leave mark in corners and make horrible noise.



Do lead-ins and outs feature or forget them for the minute?

Well they are all part the process really so should happen anyway. For instance you'll ramp into pockets for roughing to safe tool wear but radius arc into the Finish pass if enough room for better finish. If cam program allows I always let the lead out go slightly past the lean In point as well to remove cross over point.

Davek0974
15-03-2016, 03:48 PM
Thanks, lead ins and outs pretty much like the plasma then.

Radius makes sense, already use the different rad rule on the Bridgeport as that can get a bit vocal when it wants to;)

Will apply to this as well, I was going 5mm rough and 2mm finish which fits ok i think, don't really want to go below 2mm unless really needed, but there are some features that are 2mm on the job so can't use bigger.

Been researching fluids and seems pretty much anything goes, even Methylated spirits, but paraffin and oil mix seems popular - pretty much WD40 without the waxy residue ;)

New power supply arrived today, will test it out tonight ;)

JAZZCNC
15-03-2016, 04:14 PM
Will apply to this as well, I was going 5mm rough and 2mm finish which fits ok i think, don't really want to go below 2mm unless really needed, but there are some features that are 2mm on the job so can't use bigger.

Unless Rad is critical then it's worth changing rad in Cad just 0.1mm makes difference to small tools and in most cases doesn't make jot difference to part. When designing I nearly always make my none critical rad's 0.1mm over size for this reason because most tools I'm using are round numbers.

Davek0974
15-03-2016, 06:34 PM
Good point, thanks

Davek0974
16-03-2016, 08:48 AM
On the left side of my part in the OP, there are three slotted holes on the diagonal face.

After roughing the outside with a 5mm tool, these will obviously not be cut, but with my plan to finish-pass the outside with the 2mm tool in one pass, this will mean the 2mm tool taking the full depth cut on these features.

Calculator shows speed for finish pass as 996mm/min as it's only taking 0.1mm off but here it shows speed as 380mm/min as full depth slotting cut.

Options -
run all outside at the slower rate,
run outside as multiple pass contouring at the higher rate,
try and get jiggy with path rules / action points in sheet-cam to slow down in that area,
something else??

Ger21
16-03-2016, 11:31 AM
Rough cut the 3 slots in multiple passes before making your full depth perimeter cut.

Davek0974
16-03-2016, 12:04 PM
But how to just rough the 3 slots?

They are 2mm wide with a 3mm loop at the base, I was going to go in with the 2mm finish tool.

Is it as simple as defining a second pre-finish pass with the 2mm tool but still leaving the same allowance after?
But then that would not fit into the slot as its 2mm tool in a 2mm slot + 2 x 0.1mm allowance.

Or are we saying go down to smaller tool?

routercnc
16-03-2016, 12:49 PM
Hi Dave,

If Sheetcam can do isolated lines as paths then ignore the next bit -
I done something like this before and due to the limit Cut2D features I had to copy the dxf outline of the complete shape into a new CAM file, then used line creation and node editting tools to create a local closed off feature just in that area. Then deleted all the rest of the profile. So you end up with an enclosed local shape using the existing slot/loop features, plus some lines around the outside to make it enclosed. These extra lines are drawn in the scrap area outside the part. You can then select this little profile and do an inside roughing or finish pass to save running round the outside of the whole shape each time.


As the slot is 2mm wide, and using <2mm cutter could be risky, it sounds like you will have to go straight to the finish pass. You could cnc spot drill the centre of the 3mm holes in the loop, then pistol drill dia 1.5mm freehand (as material is thin you should stay inside the hole boundary!) to relieve some of the cutting.

Ger21
16-03-2016, 01:55 PM
I've never used SheetCAM, so can't help you there.

What I'd do is draw duplicate geometry for the slots, and put them on a separate layer. Then just cut them by themselves first.
Your perimeter cut can then either go into the previously cut slots, or go right past them (if you edit the geometry).
Note that some CAM programs won't let you cut a 2mm slot like that with a 2mm cutter. You may need to enlarge it to 2.01mm
AN alternative is to draw a straight line down the center, and cut a "rough" slot on the line.

Hope this makes sense.

Davek0974
16-03-2016, 02:23 PM
I'm glad i titled this part as fairly advanced ;)

Sheet cam can't isolate parts of paths, only complete entities.

I have taken all the 3mm holes off the job now and will use a steel drilling jig to drill them as a second op, five of them must match up with another part that is drilled and tapped edge-on a strip of 5mm alu so this part must be jig-drilled and to make sure holes match both parts get jig drilled.

That also speeds up the time on the mill.

It seems i have 3 options now,

1 - remove the loops at the ends of the slots and jig-drill after, cutting just a straight slot

2 - as suggested, create a duplicate part of just that area and cut between roughing and finish passes.

3 - Create a new layer and put three straight slots and smaller loops on the ends on it and cut that between rough and finish passes, allowing the finish pass to take the loops to final size.

I think I would try opt 3 as a first go, seems to make most sense to me - 3 short slots opposed to a larger path.

JAZZCNC
16-03-2016, 02:40 PM
Several ways to do this and my way would be just like gerry's with operation just on that area before doing the final finish pass. Cam software makes how easy or hard this is to do but if you Cam program that is restrictive then it's easy enough to draw in geometry soley for the purpose of Caming the part.

Like said before it's just knowing the Cam software and thinking a little differently to how Cam program might want to do it.

Davek0974
16-03-2016, 02:45 PM
Its my brain thats limited i think ;)

Messing with various ideas now, as you said, thinking differently to get the job done that matters.

Davek0974
16-03-2016, 03:44 PM
Thanks guys, it seems the best way is indeed to duplicate that small area onto a new layer, convert it into a complete entity and cut as a separate process before the finish pass.

I tried a few other options and none seemed to work correctly due to the odd shape of the slots but I think this method will do it.

Certainly getting some practice at the CAD and CAM stages anyway ;)

Davek0974
16-03-2016, 08:13 PM
Seems to work in simulation, all the steps now make sense and total time in Mach3 was about 6m plus a tool change, not bad I think. :)

How do you figure plunge rate? Same as cut, half as much etc??

Its fascinating seeing the difference in manual machining and CNC, a real eye opener and I haven't even got to cutting a part yet;)

I settled on 0.6mm DOC for the 2mm tool when pocketing the fine parts and 2mm DOC on the 5mm tool for hogging out the holes and roughing outside, then the final pass on the 2mm tool at 4.9mm DOC.

I have high-helix carbide tools listed as suitable for aluminium etc.

Hopefully good to go as soon as she's finished :)

JAZZCNC
16-03-2016, 09:45 PM
How do you figure plunge rate? Same as cut, half as much etc??

Think you know this already but if at all possible then don't plunge ramp or spiral into material. In Both cases you want to enter quickly possible to stop heat building up in tool so use same feedrate. If you must plunge then 50% feed.




I settled on 0.6mm DOC for the 2mm tool when pocketing the fine parts and 2mm DOC on the 5mm tool for hogging out the holes and roughing outside, then the final pass on the 2mm tool at 4.9mm DOC.

When doing the pockets I'd spiral down full depth 5mm and cut full depth with 40% step over. Why waste the flute length.?

Davek0974
16-03-2016, 09:55 PM
Thanks Jazz, all noted.


Dave

Davek0974
17-03-2016, 09:40 AM
Manual tool change...

I have set sheetcam to park the tool at Y0, X150 which brings it nicely to the front and centre.

Mach3 seems to lock the axes when tool-changing so how to handle the Z axis ?

When parked the Z is at my rapid height of 20mm above the material, but it looks like the park commands are in work coordinates not machine coordinates so telling the Z to go to say 100 would not work if i have less than 100 spare (thick workpiece etc) If it was in machine coords, i could tell it to go to Z0 but there is no G53 in there.

Whats a good way to get the tool to go to machine Z0 for manual changing ?

:)

Davek0974
17-03-2016, 10:42 AM
Sorted :)

Use Job Options -> ToolChange -> "run code before tool change" box and enter

G53 G1 Z0 F1500

or

G53 G0 Z0

Works perfectly

Davek0974
17-03-2016, 12:58 PM
Question...

Truing the bed surface.

In the wood forum it seems common to run a facing cut over the whole spoil-board to ensure the face is true to the tool, but what goes on when you have an aluminium bed plate??

Try and face it true, assuming you can traverse the whole plate ?

Try and shim the bed true using measuring equipment - DTI's etc.?

Something else?

JAZZCNC
17-03-2016, 01:51 PM
Dave you do realise you can jog machine to any where on the table between tool changes. You don't have to have the G-code do it.?

Regards the Bed then shim it tooling plate. Thou I think you'll find you may end up using a spoil board more than you think. For anything other than precision jobs that must have perfectly flat surface it's much easier to screw or stick material down into something like MDF or Ply. Clamps are ok but they don't always suit the job so what do you do then when can't clamp or find hole in Matrix of holes.?

Davek0974
17-03-2016, 02:03 PM
Thanks Jazz,

I did not realise as I am doing most of my debugging and research on my laptop which has no motion output etc - just a laptop and Mach3 etc. I tried 'jogging' when in tool change but it did not move so assumed it was fixed for some reason, probably just did not move as it has no motion attached. :)

I will find out this weekend what my parallel is like, I would never guess it would be perfect though, so shims is the way I would choose too.

On the bridgeport i've used many odd ways including cutting a pocket into scrap aluminium, bits of plastic, wood, basically anything goes that will hold it down. Most of what I'm planning will be 5mm Alu sheet or thinner so pretty easy to mount, DS tape would likely work if i degrease the faces.

Just trying to amass as much info as i can before I go throwing metal and cutters at it :)

Ger21
17-03-2016, 02:13 PM
When running Mach3 without the parallel port driver installed, a lot of things don't work correctly.

Davek0974
17-03-2016, 02:30 PM
That explains it then, thanks.

JAZZCNC
17-03-2016, 02:38 PM
Dave do your self a Favor and Buy Gerry's (Ger21) Screen set and make touch plate. Worth every penny and will save you hours of messing around with setting Z height etc. Much much nicer than 1024 screen set.

You'll find link at bottom Gerry's post.

Davek0974
17-03-2016, 02:43 PM
Done, looks very nice indeed.

Do you get commission ;)

Thanks

JAZZCNC
17-03-2016, 02:49 PM
Do you get commission ;)

You kinding the Man has helped Me(and 1000's others) so much over the years I'd need to recommend him to million users before got near to being worthy of commision...:encouragement:

Davek0974
17-03-2016, 02:59 PM
Some good people on here, no two ways about it :fat:

Davek0974
17-03-2016, 08:25 PM
Dave do your self a Favor and Buy Gerry's (Ger21) Screen set and make touch plate. Worth every penny and will save you hours of messing around with setting Z height etc. Much much nicer than 1024 screen set.

You'll find link at bottom Gerry's post.


Watched the videos, nicely presented and explained, looks a great screen set, can't wait to get my hands on it ;)

routercnc
17-03-2016, 10:12 PM
Been using it for ages as well and it's well worth it.

The probe function page is great with everything you can think of.

Just watch your monitor size - mine is 15" and the fonts can be a bit fuzzy. This is explained in the link and there is a preferred monitor/resolution size if I remember correctly. Even fuzzy it's still a good screenset.

Ger21
17-03-2016, 10:29 PM
Turn off Auto screen enlarge and they won't be fuzzy. I use an old 15" monitor myself.

Davek0974
18-03-2016, 08:09 AM
Arrived last night, looks money well spent, nice one.:thumsup:

Day off today, out in the shop, get the thing going :)

Davek0974
21-03-2016, 11:41 AM
This 2010 screen-set is nothing short of brilliant!

A couple of questions...

Workflow, does this seem correct?
Mount the work,
Mount Tool 1,
Set X&Y zero position,
Run initial auto zero,
Cut job.

Probing...
What is needed in order to use the X&Y probing routines - what is the 'probe'?

Tools...
If tool 2 is longer than tool 1, will it hit the fixed probe plate?
i.e do we need to try and get the tools similar in stick-out?
Not tried this yet - just looking to learn.

Thanks

Ger21
21-03-2016, 12:11 PM
The "probe" is usually the tool. Actually, to use the screenset as is, it needs to be the tool.

Make sure that you set the Clearance Plane to a high enough value so that all tools will clear the plates, and buy a safe margin. There's some info on this in the 2010 manual.

Keep in mind that the maximum probing distance is coded at 150mm (assuming you're using metric). If you need more, I can tell you how to change it.

Davek0974
21-03-2016, 12:24 PM
Ok, I will increase my clearance plane, manual only advises 3mm i think above fixed plate - thats what made me ask:)

The probe i am asking about is the one used when running the X & Y probing wizards - if the tool is grounded and the work (being metal) is grounded it cannot work, one needs to be isolated? Also the sides of an end-mill would not be accurate enough to probe an edge with?

I think 150mm is fine as thats all the Z i have.

Ger21
21-03-2016, 12:29 PM
I thought you meant for the Z axis tool length probing. For that, you need to use the tool, and use an isolated plate.

Davek0974
21-03-2016, 12:41 PM
Yeah I got that working perfectly, very slick ;)

It was the edge wizards I was interested in now.

Ger21
21-03-2016, 01:21 PM
Then you need to use a real probe.

Davek0974
21-03-2016, 01:33 PM
ok, thanks, will do some searching.

Ger21
21-03-2016, 02:31 PM
If your probing to an edge, you can use an isolated plate along the edge and specify the plate thickness. Then just use a precision dowel to probe with.

Davek0974
21-03-2016, 02:46 PM
Interesting idea, thanks.

Davek0974
22-03-2016, 09:58 AM
Back to my OP, still working out the niggles...

Where i am roughing with the 5mm tool, i have 2.5mm rads in all the internal corners, the finish tool of 2mm will plough into these at full speed - recipe for breakage here ??

Where we sorted the three slots out on the left with the roughing passes on the small tool, would it be better to pre-finish pass the whole part with the 2mm tool to bring the corners down to 1mm rads+finish allowance and then run once round with the finish pass at full depth??

This would mean i get rid of the fiddly pre-finish op on the three slots as they will come under the new full pre-finish runs. These runs would be contouring at 0.6mm DOC per pass.

I recall JAZZ mentioning it should be ok on page 1 but having seen a 2mm tool now, it seems a heavy cut on the full height of the tool??

17993
The green section plus the portion from the base of the 5mm circle etc. plus an extra 0.1mm finish allowance (not shown)

JAZZCNC
22-03-2016, 04:01 PM
Where i am roughing with the 5mm tool, i have 2.5mm rads in all the internal corners, the finish tool of 2mm will plough into these at full speed - recipe for breakage here ??

Well first you'll finish at lower feed than roughing and because of the Rad the stress on the 2mm tool is progrssive with the highest stress being fraction of the cut.
Give it big blast of lube/air when entering corner and it will fine.

Davek0974
25-03-2016, 03:31 PM
Oh well, not there yet:upset:

I spent a while assembling a fogless coolant thingy, plans as found all over the 'net, pretty easy build, seemed ok.

This was my setup - pre-drilled the cut-to-size plates so i had a fixed position, jig style setup.
18018

First run was at FS calc speeds, new 5mm high helix carbide tool, that ended up in a right mess very rapidly, boy did it complain! The fact that it managed to carry on ripping through the metal with a fully loaded tool was quite impressive - tough little some-bitch this machine!

The tool did not break!

After the "what the f*** was that?" moment passed I hit the e-stop! On examining the aftermath, it appears the new coolant system stopped the coolant and was just on air only, this allowed the tool to load up and that was the end.

After an hour of messing i got most of the gunk off the cutter - that stuff was welded up!

18019

Upon removing the plate from machine I could see the carnage below, the load-up had pulled the tool from the collet and happily chewed my nice new bed:upset:

18020

I cleaned that up with a flat file and tried again. Same cutter but this time I altered the parameters from one ramped full depth roughing pass to stepped multiple passes of 0.81mm at 1500mm/min.

I also cranked up the coolant but it sucks big time and is the typical fogger system that i did not want - the whole room filled with oil/paraffin mist, I can still taste it! Totally unsuitable but i pressed on as i did not want to be beaten on this.

I got a video of it roughing out - https://youtu.be/A9ZqR9chMwg

Things seemed a bit happier, fingers were crossed.

Then came final pass on the 2mm tool - again nice new solid carbide, the small holes were run at 1000mm/min at 0.62 DOC, ramped - these worked perfectly and i was impressed here.

The pre-finish on the three loops at the bottom again worked perfectly.

The final pass on the outside edges was at full-depth and 0.1mm cut, 1000mm/min - this is where it all fell apart again - the corners of the cutouts where the larger rads were left made a bit of a squeal but first cuts worked ok, the left side of the main part cut ok on one side of one notch but the second broke the tool and that was it for the day.:miserable:

18021

I had ordered spare cutters but some were crap and had to go back, that left me with just one 5mm and one 2mm from another supplier - the 2mm is trash and the 5mm is still gummy after about 1mm depth.

The final part is above - onion skinning will not work as there is a slight variation in bed heights and the part cannot be removed fully. I think tabbing and a sacrificial sheet of hard card or something under the plate will work better.

I also have an odd issue where mach3 went into reset when on the line before a tool-change - it would stop the spindle, lift up to clearance height then sit there in reset, pressing reset again allowed the spindle to come to park position for tool-change and then carried on normally. This happened a few times. My only suggestion here is interference from the M05 spindle-stop triggering the reset and this stopping the code right before the M06 command. I have a filter for the VFD and will bung that in.

So, unless I can find some tooling in the Bridgeport cabinet, I'm stuffed for the weekend.

I also need a coolant system as paraffin mist must be bad for health, it certainly tastes like crap!

routercnc
25-03-2016, 05:10 PM
It's easy done when you start cnc machining (and from time to time when you've been doing it a while)
You need to get used to the machine and dial it in accordingly. You'll get there

I've been machining a number of parts recently and have supported the work piece using parallels (on their side) to lift it slightly off the bed. Then pushed a piece of thin MDF under the work to reduce the vibration. The parallels keep the work flat relative to the bed and you can cut at least 1.0mm through to make sure it is free without hitting the bed. I used tabs to hold it.

Just before each pass (when it is ramping down) I vacuum around the profile to clear the previous chips and give a bit of WD40 spray and repeat until done. I don't have a compressor so this is my way currently

Good luck with the fog buster development as I think that is a good long term approach

Davek0974
25-03-2016, 05:48 PM
I'm not getting any more tooling from eBay, just ordered some 2mm and 5mm single-flute carbide tools, more swarf clearance and a stiffer tool, from Cutwell - part E5E47020 was one of them. Recommended for Aluminium and plastics.

The previous eBay ones I ordered three 2mm high helix 6mm flute, I got one that was 5mm long and two others of a random length and unknown but obviously wrong helix angle, they refunded them but it left me short on cutters.

Hopefully I can find some tooling in the cupboard to get me going again of the weekend.

As for the coolant, i'm going to drill out the jet from 0.6 to 1mm and try that - it should lower the air velocity and increase droplet size hopefully.

There is one other remote possibility - Aluminium warehouse have goofed up again and sent a soft grade of alu when I wanted 6082 T651, they have done this once before and i spent a weekend trying to figure out what was wrong with the plasma cutter when all it needed was the correct aluminium. :(

I will switch to tabbing as well, can't be any worse ;)

Davek0974
26-03-2016, 12:30 PM
Been digging through the cutter drawer, found loads of 3mm carbide 3 flutes, some 4.5mm and 5mm 3 flute cobalts as well plus a 2.5mm cobalt.

I isolated some of the features on my part and run them in the scrap from yesterday - i hate wasting metal ;)

I also tweaked the F & S sliders in HSMAdvisor to suit my machine rpm and also a lower feed-rate (i had not done this yesterday so it was running full production rates :concern: or at least trying).

Using the 5mm 3-flute and a 3mm 3-flute, plus the modified coolant (much better with nozzle cut off) I set some different paths and all seemed ok, 1mm DOC was quite happy on the 5mm with 30% step-over
on the pockets, the 3mm was ramped down to a full 5mm cut at 0.1mm deep and that seemed ok too, the end result...

18033

4 perfectly cut features. I even got a bit of video.. https://youtu.be/uIuylK4Y7qs

Annoying bit is that I can't try cutting a real job as the job is designed for 2mm finish tooling and it fails in CAM if i try using the 2.5mm cutter so I will have to wait until new cutters arrive now.

I think the single flutes will do well - lots of chip clearance and slower feeds. I have also re-cammed the job for full cut + 0.05mm and added some tabs, it will be cut on a 0.3mm spacer sheet.

Davek0974
29-03-2016, 09:58 AM
Educational....

As i have ordered some cutters from a reputable supplier now, I asked them what the recommended cut specs were for rpm, chip load and feed. They instantly sent me a nice chart with it all on, feeding the data into HSMAdvisor shows up where i was probably going wrong a bit :)

Things alter rapidly when you give the calculator the correct data - i was running too fast, too deep, too much chip. Adjusted specs for a 2mm single-flute carbide would be...
18,000rpm
2.5mm DOC
600mm/min feed

I recall when i snapped the 2mm on the weekend I had it set at something like 1400mm feed and 5mm DOC :)

Helps having correct data i guess.

Davek0974
30-03-2016, 05:58 PM
Wow! This sh1t gets expensive fast ;)

This sorry saga relates to the part shown in the OP.

Waited a week for the cutters to arrive, first 5mm carbide bit the dust in 30 seconds! The speed calculated at 12000rpm and using my lookup table i set 14500rpm as my speeds are off. The cut started and as soon as the cutter ramped in about 0.5mm of the 2.5mm set the motor bogged down like it was totally powerless and ping went 10 :(

So, back indoors, reprogrammed for about 20,000+ rpm and started again on my reserve tool, all started ok, 1st pass was flinging sizeable chips across the room, ramps down for second pass and even though i set 0.4mm holding tabs in various places, the first part broke free and fell out thus ruining that bit. Thinking the cut was too heavy i backed off the feed a bit in Mach3 and let it go, 75% of the last roughing pass and the part breaks free and takes the cutter to the bin with it. It's irrelevant but thats 25 of bits in 15 minutes, plus another sheet of 5mm Alu in the bin. :( :( Talk about pissed off!

Right, observations...

1 - Is this job actually possible?
2 - is there any point at all at running less than 100% RPM - these spindles seem to have zero power.
3 - It seems to be cutting 0.2mm below the set height - I need to tweak the Z height routine a bit, set the plate thickness a bit off to lift the tool 0.2mm
4 - How thick should holding tabs be - I set 0.4mm but clearly not enough.
5 - I set 2.5mm DOC for the roughing on a 5mm bit, go less, 1mm??

Exceedingly vexed at the moment :(

Ger21
30-03-2016, 06:03 PM
3 - It seems to be cutting 0.2mm below the set height - I need to tweak the Z height routine a bit, set the plate thickness a bit off to lift the tool 0.2mm

No, you need to find out why it's off by .2mm.
It should be right on, every time.

Davek0974
30-03-2016, 06:14 PM
I will get the indicator out and re-check the steps-per setting, can't think of anything else I can do?

routercnc
30-03-2016, 06:26 PM
I use 6mm 2f carbide 45deg alum carbide bits at 12000 rpm 900 mm/ min 1.0mm DOC. Any more DOC and the motor sounds loaded and risk of gumming up is pretty high.

I also drop the feedrate manually when deep into a profile cut as the chips are harder to clear.

I often manually drop the feedrate on the first cut as the surface seems to be harder than the core. Also my ramps in and pretty slow.
I've seen others post more aggressive rates but it does not work for my machine.

My tabs are about 3mm as you are not just holding the part but stopping it vibrate on the finish pass to get the best surface finish. Means you need to cut them out with a pad saw not just push them out .

Davek0974
30-03-2016, 06:37 PM
3mm wide tabs? But how thick?

I set 2mm wide x 0.4mm thick but due to my z running low for some as yet unknown reason, they came out at 0.15 mm thick.

Sawing these parts out is going to bugger the finish, is there another way?

If not then I might have to revert to sending them out for laser cutting again but i really, really do not want to have to do that.

routercnc
30-03-2016, 06:49 PM
Sorry typo
3mm high and ~12mm long
Careful filing and sanding then scouring pad gives a reasonable finish. If you want a mirror finish with no sign of tabs then you are back to fixing the part down in the middle using any holes that are available instead of using tabs.

On occasion I've also put the raw tabbed part in a vice edge up and used the machine to skim it down 0.05mm at a time and remove the last but if the tab. You can get a very good finish but you ideally need a parallel edge on the lower side to reference to sitting in the vice. But this takes time and is best for simple shapes.

Davek0974
30-03-2016, 07:06 PM
Wow! 3x12mm thats a serious tab, really doubt it would go on these parts IMHO.

One idea I just had was to split the job into two overlapping parts and use solid clamps with a pause in the job to allow two new clamps to be set over the cut part and the other clamps to be removed. It would mean double the tooling changes but might work?

There are no holes for fixings internally.

I was using 1300mm/min and 2.5DOC for the 5mm single-flute tool.

lucan07
30-03-2016, 07:31 PM
Is it not possible to leave 2 or 3 decent tabs 12mm x 3mm on straight edges and remove tabs as final cut after clamping the parts?

Davek0974
30-03-2016, 07:39 PM
Possibly, I'm working on it now in CAD and will post when i've got to sheet cam to see if i'm barking up the wrong tree.

Davek0974
30-03-2016, 08:10 PM
Ok, lets run this up the flagpole...

This is the job - two parts. Outer line is the base metal - 5mm Aluminium, the three point down the centre are M6 screws for fixing to the bed.

Looking at it now I can pretty much see why it failed - once the last pass of the roughing cut is made down the centres there is bugger all holding the two parts to the central stub - just the centre holding tabs which were way too thin to stand up to the cut.

This is my next plan - place some full-depth tabs maybe 10mm wide where the red dots are, make all the cuts, including the finish passes, then using the 2mm finish tool add some cuts to nibble away at the tabs after maybe fixing a couple of clamps - as suggested.
18063

Doomed to failure or possible plan ?

JAZZCNC
30-03-2016, 08:19 PM
Onion Skin will work better has it holds all round and can be lot thinner.

To be honest Dave and no disrepect meant here and I know you have some experience with milling but think your kind of trying run before can walk with this.? By that I mean you haven't had much time using this machine so don't know it's capabiltys and your part isn't exactly new user friendly with those smaller cutters.

You may be better stepping back a little and work upto this part.

Also the Water cooled spindles above 12000rpm do have resonable amount of torque and shouldn't struggle with 5mm carbide tool while ramping only 0.5mm so are you sure you have the VFD parmaeters set correctly.?

Davek0974
30-03-2016, 08:48 PM
That's the point - there is no all-round, which is why it failed. The base metal is only just over-size for the whole job, once the perimeter is roughed the only fixture it has is the middle strut and that only had the tiny tabs or possibly onion skin - just not enough meat.

No offence taken JAZZ, speak your mind ;) There is a long story with these parts, not for here but suffice to say I have customers waiting and really wanted to get them done myself instead of farming them out - this has applied some undue pressure but I think I can win still.

My experience is all manual - I'm used to throwing in a 1/2" cutter, clamping the metal down and diving in at full depth and adjusting the feed to suit as I'm twiddling the handles. The learning curve here is staggering, my presumptions were originally to use a feed and speed guide - set those parameters and have at it - this was wrong by a long-shot and I realise that now. It probably explains why 90% of the videos i have seen on youtube are all running very light cuts.

There is a slim chance that the loss of power on the spindle is connected with my odd VFD issue - maybe it really is a duff VFD after all - the new one should arrive tomorrow and i'll be fitting that before running any more tests - another good thing with a UK supplier is that help is only a call away and they are very helpful ;)

I will get that set up, check my Z axis calibration, then run some simple tests on scrap before diving in again. The new cutters will be here for the weekend and I will switch to a more softly-softly approach to feed rates as it seems most others do.

JAZZCNC
30-03-2016, 09:06 PM
The new cutters will be here for the weekend and I will switch to a more softly-softly approach to feed rates as it seems most others do.

Not too softly and most do cut too slow or too shallow but it's good idea to find your feet first before gunning it. When your settled you'll be surprised how much you can push the limits with right tooling and feeds etc.

If part has decent area to it then Double sided tape can work well if your not using cutting fluid or light amount of fluid.

Davek0974
30-03-2016, 09:16 PM
Will try the DS tape, good point.

Would you agree with the "few heavy tabs and remove last" idea??

Boyan Silyavski
30-03-2016, 09:38 PM
I wonder how you take so brave cuts and meanwhile try to tune your mist system....:boxing:


Why just you dont cut a 50x50 mm pieces and figure there the speeds, feeds and mist system.



Here are some tips, you could say cornerstones:



-mist system tip should be 0.8-1mm, 2-2.5 bar pressure at reservoir, mist spray length should be 80-100mm if all done correctly. when done correctly it will blow away even when 20mm bit cutting



About the cuts in aluminum. you will continue to snap bits until you don't figure what are you doing. Deep slotting is a recipe for disaster. Make slot double wide so you have space where the chips to go, or go slower.


Start from 12000rpm and ~600mm/min, slowly rise speed and look about the quality of the cut/6mm 2 flute/. But not on big pieces. Make small pieces and test all untill happy, including final slot depth test.


And better more mist than not at all

I leave 4mm thick by 10mm long tabs

JAZZCNC
30-03-2016, 09:43 PM
Dave this what I meant when said Aluminium bed is Ok but often you'll have Spoil board on it. So here's what I would do.
Fit spoil board that can be screwed into and surface it. Then I would change the Code and move the smaller part in wards and drill holes put screws where I have black circles on your last pick.

Then onion skin the both parts with about 0.3mm. Doesn't matter the large part will not be held down one side the rest will old it.

The skin then just breaks away and quick cleanup with De-burr sorts what's left.

I do this type thing all the time in shity 1050 2mm plate and works perfectly.

18066

Davek0974
30-03-2016, 09:58 PM
Points noted Boyan, BTW the coolant is working nicely - the cutter was clear even during the heavy cuts.

Jazz, the two screws in the small cutouts - they would be fitted after the finish pass on this features?

Spoilboard - MDF?
What sort/size for facing cutters?

JAZZCNC
30-03-2016, 10:05 PM
Points noted Boyan, BTW the coolant is working nicely - the cutter was clear even during the heavy cuts.

Jazz, the two screws in the small cutouts - they would be fitted after the finish pass on this features?

Spoilboard - MDF?
What sort/size for facing cutters?

Yes screws with washers in cut outs after finish pass on pockets.

MDF, ply anything that can screw into really.

Facing cutter then widest you have but with such small piece then wouldn't take long if small.

JAZZCNC
30-03-2016, 10:08 PM
Actually to be honest dave if spoil board is resonably flat then just for this job won't even need surfacing because your only profiling. The main reason I said surface is because 0.3mm isn't much so can easily cut thru if not flat but if you want to have thicker skin then don't bother with surfacing.

JAZZCNC
30-03-2016, 10:11 PM
Disclaimer here .!! . . . You'll need to sort that discrepency in the Z axis if your having 0.3mm Skin so don't blame if your Z isn't fettled.!

Davek0974
31-03-2016, 07:14 AM
Disclaimer here .!! . . . You'll need to sort that discrepency in the Z axis if your having 0.3mm Skin so don't blame if your Z isn't fettled.!

Thats task no1, I will re-check it with the dial indicator as i cant see how it was going too deep. I know the bed is 0.1mm out of parallel over ints 400mm length but this was too deep at the point i set the tool using my probe plate.

My thinking is that I can set a tool, set zero height using the touch-plate, command G0 Z0.00 and run the cutter over the bed without any more than a witness mark?

The only thing i can see is the steps-per being off in Mach settings.

No2 job is fit and program the new VFD for sensors vector, might help a little, should certainly sort out that odd voltage issue on the 0-10v control, maybe even the lack of power at half speed.

No3 job is to run some tests on small scraps - i seem to have plenty now ;)

While doing all that I will be resigning my parts and maybe ordering some larger sheet stock so that it can be fixed down around the edges easier.

Davek0974
31-03-2016, 06:42 PM
Getting beyond a joke now :(

Being smart ;) I programmed the new VFD at work on a test motor, all went well, nice and easy.

Just about time to fit it when i got home, booted the pc up, pressed the reset button to power up the VFD/spindle and pop goes the breaker.

Reset the mcb, try again - pop.

Ok, thinking there might be another issue here i disconnected the VFD and put a plug on it and plugged in directly - pop.

Now, this is a 32A circuit and I really can't see why a small drive like this should need a slow breaker?

Obviously no time left in the week now to replace the drive, so its a case of putting the dodgy one back now and keeping my fingers crossed.

I have emailed the supplier as they were shut by the time I came in from the shop.

Things shouldn't be this damn difficult, doing my head in now ;(

lucan07
31-03-2016, 07:10 PM
Busy time of day so, do you're breakers have an undervoltage trip? If so, something heavy starting up might be causing a dip sufficient to drop the breaker out!

Additional thought, VFD's generally default to a very fast ramp-up time, people never turn it down sometimes fixed just by changing the ramp up time.

Davek0974
31-03-2016, 07:14 PM
Doubt it, just the bog-standard 32A MK mcb.

Boyan Silyavski
31-03-2016, 07:33 PM
Same thing happened here when i was testing my belt grinder, the vfd and the 3kw motor. At the end i had to open the VFD and say "bye bye" to 6 capacitors which were connected to ground. Desoldered them and now all is allright. That with the Siemens micromaster 420. Luckily the Toshiba inverter have a button to lift the capacitors from ground in urban scenario.

To check if that's the case you just check using V meter if you have leak voltage on ground pin. Carefull!

Davek0974
31-03-2016, 07:40 PM
I don't think it's earth current, the breaker is not an ELCB, just a plain MCB. The whole shop is run from an ELCB and that did not blow.

I also can't risk opening it up, it's brand new and if it will not work here, it will have to go back.

Davek0974
31-03-2016, 08:11 PM
All is not lost ;)

Just had a reply from the supplier - that's what i call customer service!

Hidden away under a little plastic cover is a lever - pull it and it disconnects the internal EMC filters, he thought it worth a try. Popped out to shop, pulled the thingy and plugged it in - hey presto it powered up :)

Sounds like the same setup as Boyan mentioned above.

Didn't have time to run the PC up or start the spindle but at least the breaker didn't blow. I unplugged it, waited a minute and tried again and it worked ok again.

It's a promising note to end the day on at least.

Also have the new 5mm cutters - brilliant service from CutWell Ltd. Now I just need time, it's in short supply at the moment;)

JAZZCNC
31-03-2016, 08:42 PM
I had same problem with mine but unfortunatly only just seen post else could have saved you some pain. . .:joker:

Davek0974
31-03-2016, 08:49 PM
Very odd, I have two other VFD's in the shop now, once upon a time I had five on various machines, none caused this issue.

Maybe the issue is worse on newer drives with tighter EMC nonsense - the others are about 5 years old.

Hopefully get cutting again Saturday, have a little test piece lined up, got to sort the z axis calibration out first.

Davek0974
01-04-2016, 07:42 PM
RESULT (at last) :) Double whammy tonight :)

I had 20 minutes tonight and also had a chat with the VFD supplier this afternoon...

Double-checked my settings in the VFD and following advice from the tech guy I run an autotune sequence with everything connected up - apparently this is 100% vital with sensorless vector drives.

Huanyang vs Schneider Altivar... Like comparing apples and grapes!

The spindle sounds much smoother and quieter, draws less current too! No annoying resonance effects at certain speeds either. Success 1.

Happy with the way it was running I reached for the tacho in the hope that the speed ranges would be better, well they were, a tiny bit anyway but not enough for me!

I visited spindle pulleys again and raised the minimum speed to 6000, the result was that made my calibration worse, much worse - this gave me the light-bulb moment of realising that if lifting the minimum above zero makes the issue worse then surely taking the minimum BELOW zero would make it better - and oddly enough, it DID!

In the end I have a minimum spindle pulley of -6,500 and a maximum of +24,000 - I now have calibrated speeds from 8,000rpm to 24,000rpm to within about 200rpm of the requested speeds from Mach3 - success 2.

Next I thought i'd see if it had any power - called an S100 from mach, and gingerly tried to stall the spindle by hand - this was easy with the Huanyang drive, but I tried as much as i dare without risking injury and could not get it to stall or even change speed much! OK, so running at 100rpm is unrealistic - it uses more current, and likely won't do the spindle much good but knowing VFD's a little I know the power is usually naff at low rpm's.

So, at this stage at least I would say it's in far better shape now.

Tomorrow hopefully should be recalibrating the Z axis and starting test cuts again. I might even risk an old cutter and set the speed at the correct value, I have a feeling it will work this time and not bog down and break.

lucan07
01-04-2016, 07:59 PM
Now you tell me good job I like apples just brought a 2.2kw HY VFD and spindle but at 146 delivered from UK with the eBay codes yesterday i don't think I would have got near the Scheider

Davek0974
01-04-2016, 08:01 PM
146 for spindle AND drive?? thats pretty darn cheap!

The Schneider was 148 delivered BTW

lucan07
01-04-2016, 08:05 PM
Yeah saw the 20% discount for everything on eBay so had to go for it only ran from 4-10pm found a HY chinese supplier with warehouse in UK near me in Leicester so did the deal can resell on ebay for that money and still not lose so gotta be worth a shot.

JAZZCNC
01-04-2016, 09:00 PM
Now you tell me good job I like apples just brought a 2.2kw HY VFD and spindle but at 146 delivered from UK with the eBay codes yesterday i don't think I would have got near the Scheider

Don't threat I fit these all the time and think Dave had VFD which wasn't setup correctly or possibly faulty. Normally they work very well above 6000rpm.

Yes the Huanyang won't match Vector drives for torque, esp at low rpm but it's more than good enough for cutting wood an aluminium between 8000-24000rpm with smaller cutters which is where you'll mostly run it.

Davek0974
01-04-2016, 09:06 PM
I agree, I have a strong suspicion it was a duff drive - setting it up wrong would not give the odd fact that I could not get a voltage reading on the 0-10v inputs when running - that is extremely suspicious.

Davek0974
02-04-2016, 12:42 PM
Ok, getting somewhere now :)

I checked the Z axis calibration, microscopic tweak to steps-per but nothing major.

It turns out the reason my previous onion-skinning and tabbing failed was because of operator error - garbage in, garbage out! The metal i ordered was 5mm thick, I set that in CAM and tried to leave a 0.1mm skin or a 0.3mm tab.

In real life however the sheet was only 4.85mm thick - there was the missing skin and tab, I was telling it to go deeper than it really was - lesson learnt - don't ever trust what you order is what you get :)

Another possible source of error in the sub millimetre range was the probe touch-plate, it miked up at anything from 1.42mm to 1.51mm depending on where you place the micrometer. I have fixed this by scribing an area on the surface of the plate where it measures exactly 1.5mm - always using that spot should sort it out.

So, on to cutting stuff, I threw in my sacrificial 5mm 3-flute HSS cutter and set a lump of my 4.85mm ally on the bed.

In CAM i made a straight line 40mm long, 4mm deep, slot width, plunge in, 1mm DOC, speed at 8000rpm(where it bogged down before) and feeds ranging at 600, 800, 1000, 1200mm/min.

Result was perfect in all settings, no speed drop at all, perfect cuts.

Next test was the same job but this time 1.5mm DOC per pass, same speed ranges.

Result was 100% perfect, it didn't even know it was cutting!

A video of a 1.5mm DOC 1200mm/min, 4mm deep slot cut...
https://youtu.be/cL3Om6xMfK8

So, I am now going to risk a tool and try my job again, onion skin at 0.15mm to start with, I am expecting a failure as I don't think the sheets are really big enough for the job but who knows :)

Davek0974
02-04-2016, 03:37 PM
Made it's first full-job :)

Yes, I know it's a failed part - i lost a cutter due to it hitting a hold-down bolt caused by my messing with the CAM so much I forgot which file was which :distress: I didn't want to add wasted metal to a wasted cutter so i reset the file and cut the next run over the first one.

18069

Onion-skin was perfect, too thick and hard to remove at 0.15mm but i did manage to take the job right through all the post-finish drilling, counter-sinking and fettling just to prove the process.

OK, education time...

Poor quality on the finish passes, 2mm single-flute cutter, 0.6mm DOC, 450mm/min cut, 23,000rpm - chatter I think.

18070

How to improve?? It looked better on the roughing cut ;)

Videos...

Roughing cut...
https://youtu.be/oSgf-0C5PHM

Pre-finishing the fiddly loops, 2mm tool...
https://youtu.be/nD4If43P3c0

Job took 43 minutes including tool-change, mostly the delicate finish cuts, I will look at these a bit more as something is off a little there I think.

Any pointers?

On the next run I'm going to take the skin down by 0.05mm and also put a sheet of paper or card under so I take the fine detail - holes and slots, down to 100% depth.

Boyan Silyavski
02-04-2016, 06:31 PM
The pointers: i said it many times, and most disagreed. For perfect aluminum finish if the machine is normal, that combo gives me the best finish. I don't care about 12k rpm or 30 krpm. That combo for 3mm bits gives me best finish. On the yellow machine i could cut at 12krpm and 2500mm min at 1mm deep with 1/4 bit. But best perfect finish is around 600mm min/ hence 25 ipm/

18071

Davek0974
02-04-2016, 06:47 PM
Those settings are not far off where i was, I was a little slower feed and faster rpm, that may make a difference, don't forget there is a fair bit difference between a 1/8" and 2mm tool.

Thoughts over dinner...

1 - Make the final pass on the main parts with the 5mm cutter then isolate the small features and machine only those bits with the 2mm tool?

2 - Try the final pass with the 2mm at full depth but add a slow-down in the corners where it's biting the rads from the 5mm tool?

3 - something else?

routercnc
02-04-2016, 06:56 PM
On the finish pass question - I don't often use small cutters so don't know what the problem is. But 0.6mm DOC seems small for the finish pass ?

I generally use 6mm cutters and for finishing I leave 0.1mm roughing on the part - how much are you leaving?. Then I cut at 3mm DOC as this works well but I could probably do anything up to 10mm DOC as you're hardly removing any material on the finish.

Here is the finish on a 10mm part using this method:
18072

Davek0974
02-04-2016, 07:07 PM
I left 0.1mm from the roughing pass.

The 2mm cutters are spec'd to 3mm DOC but I still have concerns where they hit the rads from the 5mm tool and also have to plough into the corners a bit to create the sharp internals. Maybe my option 2 above would work?

Davek0974
02-04-2016, 07:39 PM
Looking at figures there is a fair difference between the finishing pass and the sharp corners -

Lets go for a 2.5mm DOC this time, just below the cutters limit and half the final depth...

Finishing the edge wants 23,000rpm and 670mm/min feed
Ploughing out the rads and creating the sharp corners - basically a slotting cut - wants 18,500rpm and 180mm/min feed

So quite a change, all other parameters being left fixed, sounds like a path rule in SheetCam might work there?

That would be a 25% speed reduction and setting feed to 28%.

Davek0974
03-04-2016, 01:59 PM
The machine made it's first saleable parts today :)

I did sacrifice two 2mm cutters, here's how...

On the part in the OP, there is a little square notch, first from the left along the top edge, it's about 4mm square and as such was not roughed out by the 5mm tool on the first pass. I set the code for a 2.5mm deep cut on the finishing pass with the 2mm tool and added a reduction to feed with CAM rules, it worked nicely until the tool reached that notch when it died.

I then increased the before and after feed change in CAM so the rate slowed well before and after the notch - ping went another tool. I then reverted back to 0.6mm per pass and 450mm/min rate as before and it sailed through. Still got that slightly poor surface finish though.

So, it seems despite what HSM says, even on severely reduced settings, you cannot slot 2.5mm deep with a 2mm tool.

Now, in light of the slow finish passes and the fact that it did seem to handle the 5mm rads with a CAM rule and 2.5mm DOC, is it worth singling that feature out and running a pre-finish run on it like I did with the loops??

Apart from that, I'm not happy with the paraffin/oil mix, seems to be affecting my hands a bit, I have found a suitable retail item - MilliCut J40 from Cutwell, its a veg oil based product.

Has anyone got there mill in an enclosure? I'm finding the floor is covered in chips about a 4' radius around the little bugger from the roughing passes - the 2mm tool just makes dust.

lucan07
03-04-2016, 03:24 PM
The machine made it's first saleable parts today :)


Next step get the processing nailed down and make them profitable too, let the bugger start earning its keep!

Davek0974
03-04-2016, 04:09 PM
Yep, already on that ;)

I just revisited the original plans for the part with the notch in it and it appears it's non-critical so I have altered it from 4mm wide and square to 5.1mm wide and half-round so the roughing tool will rip out most of it and I can try the 2.5mm DOC on the finish pass again - the 0.6mm cuts were where most of the time was eaten.

While it was running today I was also making other stuff so the time taken is not critical to a tight degree, once I get going I can finish one set of parts while the next is running - there are holes to drill and tap etc. Demand is not massive for these but crucially it means I don't have to send them out for laser cutting anymore.:unconscious: :cheerful:

I can also move another part I make from the plasma cutter to the mill as the quality is higher and finishing/clean-up time would be far less as plasma leaves a very rough edge on aluminium.

Just need to sort out a better bucket for the cooling water, possibly some sort chip management, and some better cutting fluid.

I might also try some low-speed tests just to see how low she can go.

lucan07
03-04-2016, 04:28 PM
As regards your enclosure I don't use an enclosure as such but have screens in Acrylic for certain jobs to control chip/coolant ejection etc, very easy to cut and weld together using Dichloromethane.

I should mention got a great deal on load of 5mm acrylic, less than 30p a square ft.

JAZZCNC
03-04-2016, 09:22 PM
I can also move another part I make from the plasma cutter to the mill as the quality is higher and finishing/clean-up time would be far less as plasma leaves a very rough edge on aluminium.

I would combine them and let the Plasma rough them out and finish them with the router using full depth finish pass. May need a Jig if cutting lots but will be worth the time to make in long run.

What's Max thickness Ali can you cut with plasma.?

Davek0974
03-04-2016, 09:39 PM
Hi Jazz,

Can't combine, one is 5mm and the other is 3mm plus the bed is too small to take both parts ;)

The parts i have been getting working in this thread were never plasma'd - too much detail and the heat would warp them, laser cutting does distort but not as much, costs though - that's why I wanted to bring them in-house.

I could pre-cut the 3mm parts on the plasma, would save metal as i can only order square-cut sheet or blanks and these parts are triangular. Would then need to be a two-step fixing on the mill - fix through the internal aperture wastage and cut the outside then fix clamps and finish the internal details. Would still work though, these are simpler parts to make.

I can plasma 9.5mm if it needs piercing or 19mm if I can edge-start the cut. It's not the favourite flavour of metal for plasma cutting though.

JAZZCNC
03-04-2016, 09:55 PM
I can plasma 9.5mm if it needs piercing or 19mm if I can edge-start the cut. It's not the favourite flavour of metal for plasma cutting though.

What kind of feedrates would you cut 19mm Ali with.? Is this using 45A plasma.?

Boyan Silyavski
03-04-2016, 10:24 PM
18088
18089

This is Kyocera carbide micro bits feed and speed chart. They are definitely one of the sharpest and overall best bits around. So if you are using inferior -30% at least on all data.

Vc - cutting speed
f - chip load or feed per tooth
Fr- feed rate mm/min
D- diameter of carbide bit
U- number of teeth on cutter
p=3.14


Ae - side removal
Ap - face removal


1.
determine spindle speed rpm/min depending an operation/roughing, slotting, finishing/


RPM=(Vc*1000)/(p*D)
so
RPM=(150*1000)/(3.14*2)=~24k RPM, so you are spot on here




2.


Calculate feed rate mm/min:


Fr=f*U*RPM
so
Fr =0.024*2*24000=1152mm/min for slotting

=0.002*2*24000=96mm/min for finishing


That all on a mill with very good cooling and chip removal. Diameter depth and 30% tool engagement

So if you play with the second formula you could easily see why you can no make a nice finishing pass. cause for 800mm/min feed you will need to have the spindle at 8000rpm, not 24000.

Now lower some percent that you ar not cutting on a mill with jet cooling the bit...

And bear in mind that the first speed calc is most probably for roughing bit, because that's how typically is done, that's why seems so fast.

From my experience there is no big science here, i have tested cuts on various machines and the only thing that really differs is the depth of cut that could be achieved with a particular machine.

Davek0974
04-04-2016, 07:35 AM
Thanks Boyan, all I do is plug the manufacturers cutter specs into HSM Advisor, set the cut details and move the feed rate to 30%.

I was not feeding at 800mm/min, don't forget my tools are only single flute.

The cut is a tricky one though as the corners are more like slotting and the rest is plain finishing so a mix of heavy and light cuts.

Davek0974
04-04-2016, 08:38 PM
If my understanding is better, after a good chat with the guy that supports HSM Advisor, it seems I might be a bit over zealous with the settings?

Plugging numbers again, I get for the 2mm tool, 18,500 rpm, 1,200 mm/min feed, 0.5mm DOC and 0.065mm/t chip load.

Reasoning - the limiting factors are the larger rads in the sharpened corners - this becomes slotting - also the manufacturers chip load limit of 0.065mm/t was set to not be exceeded, that gave DOC as 0.506mm as part of a balanced result to meet those factors.

So my earlier run was 0.6mm - too deep, 23,000rpm - to fast, 450mm/min - too slow. It survived but took a long time and gave poor surface finish.

The tool cannot give a 2.5mm DOC with any setting due to the slotting factor - the tool exceeds 100% torque limits = snapping - this backs up what really happened when i tried it.

So it seems lighter, faster is a way forwards, might risk a tool and try it I think. Its more passes but travelling at 3 x the speed so should still be quicker.

Davek0974
06-04-2016, 01:37 PM
RESULT !

Had a bit of time off work today so out in the shop :)

The new cut parameters seem to be perfect so far, the 5mm roughing cuts seem a bit off as i was seeing some chip-welding to the sides of the cut, this was at 2.5mmDOC an 1350mm/min @ 24000rpm, this was with coolant as well so its a bit wrong somewhere there, not sure if too much rpm, too much feed or something else, manuf states max rpm is 12000 so maybe i need to retune at that speed?

I made several alterations to the CAM and CAD by way of pre-finishing the sharp corners with the 2mm tool - this works great, then the final pass with the 2mm at 24000rpm 5mm DOC, 0.1mm WOC and 244mm/min feed spat out lovely little shards of swarf and not dust. Surface finish is now 100% quality.

The CAD/CAM changes also reduced my part time from 45mins+ to 20mins which is a considerable change, that includes tool change but not plate setting and bed clean-up.

Pictures later.

Davek0974
06-04-2016, 05:21 PM
The 5mm cutter runs cleaner at 18000rpm and 1000mm/min. :)

Edge finish...
18107

Nice pile of swarf...
18106

I had the onion-skin set a little too tight and had to hold the parts in for part of the finish cut but that's easily fixed.

Couple of videos...

Running the 5mm roughing cut, I can't be sure if this was the fast or slow setting though.
https://youtu.be/I_gkfQ6zJKQ

Pre-finishing the sharp corners...
https://youtu.be/h2HGya_X3iU

Still need to sort out some chip management as the mess is unbelievable ;)

Davek0974
08-04-2016, 06:27 PM
2 Jobs tested and in production :) 2nd one much less stress ;)

2010 screen-set, tool change routine...

On this job I did exactly the same as before but the first cutter seems to have run about 0.2mm lower than it should, made a bit more mess out of my bed but i'm not worried about that as it's buggered anyway ;)

The next two tool changes worked perfectly and did not gouge the bed.

Anything that can cause this?

I have verified the code and all parts are cut to the same depth.

Clive S
08-04-2016, 07:41 PM
Anything that can cause this?

Human error or the tool slipped in the collet

Davek0974
08-04-2016, 07:55 PM
Vaguely possible but why only slip 0.2mm and not just keep going as usual?

The second and third tools were spot-on which indicates the initial height sense was good, i think.

lucan07
08-04-2016, 08:06 PM
If it did slip the torque from cutting and centrifual forces or heat generated in the tool could have locked it tight again.

One plus for leaving my cast iron bed for later use if I feck up a bit of MDF or even some Aluminium extrusion I won't be to upset but I don't want to replace a 1000x700x50mm cast plate that has been ground

Davek0974
08-04-2016, 08:13 PM
Yeah i also have a cast iron bed but its only ever for use as a sub-bed, the part that has been mauled is only 15mm Eco-cast plate so i'm not bothered too much, will likely end up taking a skim off it anyway.

lucan07
08-04-2016, 08:20 PM
Only reason I didn't use mine is I don't like shredded wheat enough to eat three, or the fact that after having it ground flat advised to leave it on steel base, either part I could find a couple of mates and man handle up a flight of stairs into my flat but together they're almost 0.4 of a ton and can wait until I move again and have my workshop at ground level.

Ger21
09-04-2016, 12:27 AM
2 Jobs tested and in production :) 2nd one much less stress ;)

2010 screen-set, tool change routine...

On this job I did exactly the same as before but the first cutter seems to have run about 0.2mm lower than it should, made a bit more mess out of my bed but i'm not worried about that as it's buggered anyway ;)

The next two tool changes worked perfectly and did not gouge the bed.

Anything that can cause this?


Didn't you have this issue before?

Davek0974
09-04-2016, 08:24 AM
Didn't you have this issue before?

That was when the coolant stopped and the cutter loaded up, i was also pushing much hared back then as the feeds/speeds were off.

This job was only 3mm aluminium, I was taking a full depth cut though. Odd that it was only the first cutter, which went back in later to do a final full depth pass around the edge.

I will have a look at the shank and see if there are any skid marks.

Also have another to make today.

Davek0974
09-04-2016, 12:16 PM
Next run went fine, apart from a boo-boo ;(

I've seen this behaviour before on the plasma table - something goes wrong, you press stop on the Mach screen, I know your supposed to press feed-hold but i wanted something between e-stop and feed-hold as the coolant failed to come on (duff relay) so i knew it would load up and break and so pressed stop.

Fixed the issue, wound the code back to the last M05 stop and set next line.

Pressed cycle start and the cutter goes down where it is and shoots off to X+ at cut speed, snapping the tool off. It should have gone back to where it started last time and re-cut the partial slot and then finished normally.

Looking at the DRO's the X machine position is off by 226mm which i think is the setting that it was stopped at so now the cut start was not X5 as it should be but X-221 or something like that.

As i said, this has happened on the plasma and as here, the only way back is scrap the part, re-home and start again. I failed to note the X/Y positions for job location so i couldn't reset it and try again.

Some sequence of events throws Mach positions into a tizzy and it shits the bed. On the plasma no harm usually but on the mill = broken tool :(

Oh well, the next part finished perfectly, no bed gouging, if anything it was running too high now - the material miked up at 2.91mm, i programmed the cuts to 2.90mm and there was still a good skin left at the base. Something seems a little variable on height setting possibly?

Ger21
10-04-2016, 02:02 PM
Any time you press Stop, you MUST re-home the machine before doing anything else.
And I'd highly recommend using Run From Here, unless you know exactly what state mach3 is in when you use Set Next Line.

Davek0974
10-04-2016, 02:43 PM
Thanks for that, explains a lot then ;) Don't think I've ever used RFH...reaches for manual ;)

I think for what I am doing - small batch production - saving the offsets is a good idea??

All the raw plates are pre-cut to the same size and pre-drilled for fixing to the bed so each part will always start in the same position or work-offset.

Is that what offsets are for?

Could I then have re-homed the machine and loaded the offset then carried on with part I had stopped on??

Lots to learn....

Ger21
10-04-2016, 02:47 PM
If you don't close Mach3, the offsets should still remain after homing. (I think)
Yes, if you have a specific part that you always run in the same place, use an offset like G55,G56,G57...
Add the G -code to the beginning of your code, and save the offsets. Then when you turn on your machine, you just home, load the code and run.

Davek0974
10-04-2016, 02:50 PM
Sounds good, an offset will do what i need, i have never checked if the work position remains after a home, something else to check.

JAZZCNC
10-04-2016, 05:54 PM
Sounds good, an offset will do what i need, i have never checked if the work position remains after a home, something else to check.

Yes it does offsets are Modal so will only change if you set a different offset. G54 being default so if you don't save the Fixture offset when closing Mach3 it will always load the previous G54 offset which was saved.

Regards Homing and Stop. It actually goes further than that regards homing. If you have stopped the G-code with feedhold and in controlled manner then if you for any reason power down the drives, which a safe E-stop system should. Then you should home the machine when they power back up.?
This is because they often jump to next full Step so your then out of positon to where mach thinks it is.

Then if your trying to get back to position use RFH. I use RFH all the time it's a great tools when shit hits the Fan.!!!

Davek0974
10-04-2016, 06:07 PM
Great stuff,

If I'm using say G55 for my job, it will still be there next time i load?? That sounds like a recipe for fun ;) Can it be programmed to always load into G54?

The G55 could/should be added to the start of the specific G-Code file?

Stuff to learn...

JAZZCNC
10-04-2016, 06:31 PM
If you save the Offsets when closing or by Saving directly in work offsets then G55 will be saved but by default Mach on start up will load G54 so your safe.
If you want G55 or any other offset you'll have to call it with MDI or Thru G-code.

To use different Offset with in one G-code file you'll first need to create the offset and save it.

To see it work Try this.!!
By default your in G54 so set Zero work coordinate. Then Type G55 in MDI now jog away and set Zero again in different place.

Now in MDi Type G54 G0 x0 y0 and it will got back to zero you set for G54. Now type G55 G0 x0 y0 and it will go back to zero for G55.

So say you have one part you need to make but in two different materials. First set up the Zero Offsets for each material G54 & G55.
Then use copy and paste. The first part will most likely have G54 at the begining by default. So paste the code again for the second part and replace G54 with G55.

Now when code runs and gets to second run of part it will use the new Zero at G55.

If you want to keep thses offsets then go into Offests and save work offsets.
To be honest saving Offsets before starting job is a good habbit to get into because if Mach crashes or PC then you lose the offsets and have no way easy way to get back into position. This happens often with parallel port machines when being run hard.

Davek0974
10-04-2016, 06:38 PM
Excellent, that makes sense.

I have "optional offset save" turned off so it only saves what i want to save into the offset table.

I don't think sheetcam has a work offset option so it'll have to be a manual add, but can't have everything i guess ;)

Davek0974
13-04-2016, 07:04 PM
Hmm, back to school, two issues tonight.

Offsets, seems i have not grasped it yet or I am in the wrong work sequence...

Yesterday I saved the work offsets for my production job - G55, I also added G55 to the start of the code. I then loaded up the material, changed the tool & set my top-of-material Z zero. Pressed cycle-start and got Soft-Limits warning on Z, looking at the numbers on the DRO's I could see something was wrong.

I deleted the the G55 from the code, switched to G54 Offset, reset my tool zero just in case, set work X&Y zero as normal, and ran the job as before.

So, not sure what i am doing wrong but clearly offsets do not work totally how I envisaged them to work. Do you have to be in the correct offset BEFORE setting the tool and Z zero?? If yes then that was likely mistake No1 as I was in default G54 when I set the tool. What I expected was for the offset to only affect X & Y not Z (i think)

Z Zero, again.

yesterday the job cut perfectly, onion skin just about held it together and a nice part came out. Tonight, same file, onion skin failed as the tool chewed the bed by about 0.1mm or a bit less - this meant the part got 90% of the way and failed on the finish pass, luckily the cutter survived but the part was toast and now resides in the scrap bin.

So, I have two issues here, top-of-material setting and work-holding.

Here is the part before it went flying to the bin in a red-mist:concern:
18197

Now, after cooling down, I miked the metal up and it seems the thickness is not very reliable, the 7 bits i have left ranging from 5.05mm to 5.25mm depending where you measure it - I think this accounts for the failed onion-skinning and subsequent junk output.

My first resolution to this is to mark a spot with a sharpie, measure it, note it, CAM the part specifically for that thickness, set the tool zero exactly on the sharpie mark and try again - I do not think this is a machine error, more a material error.

Work-holding, these parts must be 100% flat and clean, if I tried adding some carpet tape etc under it, would I be able to get the part off the bed when cut?

lucan07
13-04-2016, 08:03 PM
If this is a regular job I cannot see why you do not create a jig waste board to hold material in a recess with appropriate hold downs permenantly in place so 4 nuts or so to lock jig onto bed, material in recess and locking tabs clamps (cheap chinese 120kg hold downs or similar you could have a couple to swing in after finishing pass goes by if needed and cut clean threough each time) to hold material off you go, no more biting into the bed, cutting through not going to matter occasionally one out quick vacuum next one one in, seems to me a lot of wheels being reinvented.

Ger21
13-04-2016, 08:09 PM
On my website, there are some modified macros that will zero the Z axis for all of the G54-G59 offsets at once, regardless of which one you are currently in.

As for material thickness, there's another option in the 2010 Screenset called "Material Offset". When checked, you zero the Z axis to the table, and Z zero is set at the material thickness value above the table. It's works basically the same as setting Z zero to the bottom of your material. If you are doing pockets, note that this will affect the pocket depth if the material thickness varies.

Davek0974
13-04-2016, 09:11 PM
If this is a regular job I cannot see why you do not create a jig waste board to hold material in a recess with appropriate hold downs permenantly in place so 4 nuts or so to lock jig onto bed, material in recess and locking tabs clamps (cheap chinese 120kg hold downs or similar you could have a couple to swing in after finishing pass goes by if needed and cut clean threough each time) to hold material off you go, no more biting into the bed, cutting through not going to matter occasionally one out quick vacuum next one one in, seems to me a lot of wheels being reinvented.

Ok, but if the part is finished all round that would mean diving in to fix clamps while the finish pass is running ? Or pressing feed-hold mid-cut? Neither sound good to me personally. I'm not deliberately trying to reinvent wheels, I just do what makes sense to me at the time i need to do it. The plate is fixed with the three bolts down the centre, these go through the scrap part, the outside clamps don't really do too much.

I just can't 'see' a way to clamp the parts as they are being cut.

As for spoil board then yes, if the bed was not already damaged I would fit one, this one sacrificed itself in the name of education;)

Davek0974
13-04-2016, 09:35 PM
On my website, there are some modified macros that will zero the Z axis for all of the G54-G59 offsets at once, regardless of which one you are currently in.

As for material thickness, there's another option in the 2010 Screenset called "Material Offset". When checked, you zero the Z axis to the table, and Z zero is set at the material thickness value above the table. It's works basically the same as setting Z zero to the bottom of your material. If you are doing pockets, note that this will affect the pocket depth if the material thickness varies.

Thanks Gerry,
downloaded the macro's, seems like a better system to me.

I'll keep the ref method as it is at present and try other ways of sorting it out, the bed zero method looks useful but I can see ways it would land me in trouble sometimes ;)

I am fairly certain the issue is the variable thickness of the metal, surprised me how bad it is but it does explain why the part fails sometimes.

CharlieRam
13-04-2016, 11:13 PM
I just can't 'see' a way to clamp the parts as they are being cut.

Use a M00 at a convenient point, then press cycle start to continue, spindle stop might also be good at this point :)

Davek0974
14-04-2016, 07:09 AM
Use a M00 at a convenient point, then press cycle start to continue, spindle stop might also be good at this point :)


Yes but the finish cut is one continuous cut, you don't want an M00 in the middle of a continuous cut because you will not get another lead-out and lead-in so a tool mark is going to show, let alone stopping and starting the tool mid-cut will probably break it.

Fitting clamps will mean working in the short space of time while the cutter is up the other end of the job, these parts are small so time is short and this is therefore dangerous. The Z axis mount is wider than the job so all clamps have to be low-profile <=10mm high or it means using a longer stick-out on the tool which again is not good on a 2mm cutter.

These are difficult parts to make well but that does not mean they cannot be made ;)

routercnc
14-04-2016, 07:19 AM
Hi Dave,

I tend to use the tab method but this does leave a small witness mark (although the parts are just for me so that's ok). For customer parts I can understand why you are trying not to.

So I think if I were to try the onion skin method I would skim the bed first then zero the end of the tool to the BED. Then MDI jog the Z axis up to 5.1mm (if the part is nominally 4.9-5.1 say) and then ZERO the DRO again.

In your CAM you would than ask for a depth of 5.0mm. This would leave exactly 0.1mm of onion skin. This method is independent of the variation of part thickness.

Davek0974
14-04-2016, 07:29 AM
Thanks, that sounds a very similar method to Gerry's - using his "material height" DRO. I might have a go at skimming the bed and try that out.

lucan07
14-04-2016, 07:56 AM
When I use the M00 I simply extend cut into scrap section past end of cut or put in a small loop and restart on a corner with change of direction and no signs of me doing so. think about it like cutting it on your manual mill overshoot on external long straightish edge to fascilitate later clamping, pause in scrap material on overshoot, add clamps to suit which could be pre mounted to swing over and clamp and carry on.

CharlieRam
14-04-2016, 12:21 PM
Looking at your part, there are quite a few holes to screw into a spoil board so I would have the M00 after the holes were drilled to insert some screws to clamp the piece down, then just cycle start for the profile

Davek0974
14-04-2016, 12:48 PM
Hi

yes there are some 3mm holes on one part and a couple of useful apertures but nothing at all on the second part, on the right in the picture, I can't add any holes either :(

CharlieRam
14-04-2016, 01:02 PM
OK then, complete the outer profile, m00, remove waste outer profile, clamp right component leaving room for profile cut, cycle start and finish profile cut to separate parts. Easy :-)

Davek0974
14-04-2016, 01:10 PM
Ah, now that's interesting ;)

So i would modify the drawing to make the outer edge of the two parts into a single path, then connect the inner edge of both parts into another solid path that overlaps the first path at each end, then as you say, run the small holes and the outer path to finish state and full depth, remove junk frame, add clamps to each part and run middle path to finish.

I'm liking that, thanks. It means adding another two tool changes but thats not really relevant if it ensures the parts come off in top quality AND without any onion-skin to clean up.

Nice.

Davek0974
14-04-2016, 06:40 PM
WooHoo! :)

Thanks CharlieRam, your idea worked perfectly, best parts so far and a lot less stress on the nerves ;)

I need to make some decent clamps etc but the extra tool changes were more than made up for with the time saved through not having much clean-up to do, just a quick run with a de-burrer and a little emery cloth.

Davek0974
14-04-2016, 07:00 PM
On my website, there are some modified macros that will zero the Z axis for all of the G54-G59 offsets at once, regardless of which one you are currently in.



These work much better, thanks.

Much more like how I imagined it would function :)

CharlieRam
14-04-2016, 07:49 PM
Glad it helped, If you drill the holes first, then do the pockets and outer profile, m00 etc. would that reduce tool changes?

Davek0974
14-04-2016, 07:55 PM
Not this time because the holes need the 2mm tool to get the sharp corners I need.

It works pretty smooth though, the 2010 tool-change routine is fantastic and a big help.


Of course, with a tool-changer........

lucan07
14-04-2016, 08:35 PM
Already planning Version 2.0?

Davek0974
14-04-2016, 08:44 PM
Not yet, but in the couple of years since building my first CNC plasma table, I have started to realise how cool CNC machines really are ;)

Tool-changer spindles are a bit

Davek0974
15-04-2016, 07:47 AM
Ok, getting smart here...

I want to insert a code snippet in Sheet-Cam that will run the tool to my park position (M883) and then pause for me to dive in and change the work clamps etc for the final processes.

It seems to be posting the code wrong though as shown here:



Code:


N24280 G01 X116.2500 Z-5.200
N24290 G02 X117.7500 Y70.7123 Z-5.2000 I0.0000 J-1.5000
N24300 G01 Y40.2123 Z-5.200
N24310 G02 X116.2500 Y38.7123 Z-5.2000 I-1.5000 J0.0000
N24320 G01 X104.9616 Z-5.200
N24330 G03 X103.6816 Y37.4323 Z-5.2000 I0.0000 J-1.2800
N24340 (Operation: Insert code snippet Code: Wait For Clamping Change)
N24350 G00 Z20.0000
N24360 M883 (Go to park position)
N24370 M0 (Change The Clamps Now)
N24380 (Operation: Inside Offset, Part To Cut Last, T4: 5.0mm Carbide 1 Flute YG, 5.2 mm Deep)
N24390 S18000 M05
N24400 (5.0mm Carbide 1 Flute YG)
N24410 T4 M06
N24420 G43 H4
N24430 S18000 M03
N24440 G00 X82.7074 Y370.0327
N24450 Z1.0000
N24460 G01 Z0.000 F475.0
N24470 G03 X81.4274 Y371.3127 Z-0.1054 I-1.2800 J0.0000




Unless I am wrong, this will lift the tool (line 24350) then go to park (line 24360) then pause (line 24370) BUT the spindle will still be running as the M05 is not until AFTER the pause (line 24390)??

Seems wrong and dangerous?

Looks a bit messed up but all I am doing is inserting a code snippet that has two lines :

M883 (Go to park)
M0 (Change the clamps)

Any ideas, I have posted on the Sheet-Cam forum but???

Davek0974
15-04-2016, 11:54 AM
From Les at Sheet-Cam:- you have to add the M05 as well because the post does not know what you want to insert so it treats it as text.

Now it looks like this...

N24330 G03 X103.6816 Y37.4323 Z-5.2000 I0.0000 J-1.2800
N24340 (Operation: Insert code snippet Code: Wait For Clamping Change)
N24350 G00 Z20.0000
N24355 M05 (Stop Spindle)
N24360 M883 (Go to park position)
N24370 M0 (Change The Clamps Now)
N24380 (Operation: Inside Offset, Part To Cut Last, T4: 5.0mm Carbide 1 Flute YG, 5.2 mm Deep)
N24390 S18000 M05
N24400 (5.0mm Carbide 1 Flute YG)
N24410 T4 M06
N24420 G43 H4

Seems like that will work

Davek0974
16-04-2016, 12:21 PM
The new code snippet worked well, very slick now - pauses, goes to park, tells me to change the clamps, then goes to tool-change then starts cutting, nice :)

The only odd thing i saw was that the job timer in Mach3 was reset at some stage, not sure if it was the pause or the "go to park" macro call??

Also made up some nice clamps to replace the bent bits of scrap I had on it ;)

18208

The bed does need a skim though, I have found in the tool drawer a nice 12mm inserted tip carbide cutter that should do nicely for this.

m_c
16-04-2016, 03:15 PM
IIRC the timer gets reset every time you press cycle start.

routercnc
16-04-2016, 03:24 PM
Well done looking good now

I'm sure you know the clamps are better if the bolt is at the work piece end rather than middle - slotted clamps and more bed plate holes would be a good next step when you get a moment. Good stuff anyway . . .

Davek0974
16-04-2016, 03:53 PM
Yes, thats standard clamping law - bolts close to part and back end of clamp slightly higher than part;)

They do work well though, todays part was another total success, I don't think the stress on the part is that high in this case, there is only one cut that will put it under strain - the second/last pass on the 5mm roughing tool which separates the parts from the central stub, after that it's just light tickling with the 2mm tool.

The next major issue is getting some sort of chip control round her - the mess is ridiculous.

Davek0974
17-04-2016, 08:18 AM
More questions, anyone care to put pics up of their whole setup?

I'm looking to find a home for the damn keyboard, monitor and mouse - this lot seems to take up more space than the machine! The keyboard and monitor are also suffering under the shower of chips ;)

routercnc
17-04-2016, 08:59 AM
18214

18215

Davek0974
17-04-2016, 09:54 AM
Nice, way too clean and tidy ;)

Wall mounted monitor is good, the keyboard and mouse is sort of where mine is but the chips get flung for about a 4 foot radius when cutting so i have to cover the KB up every time i press start!

I need to move it to a better location really but space is tight, or poorly arranged, or both ;)

Too much in one room really, it's 5.2m x 4.2m - CNC plasma, CNC milling, manual milling, pillar drill, lathe, power-coating station and oven, bench, pedestal grinder/buffing, Mig welder and bench, 20T press, bandsaw, metal storage, probably more....

lucan07
17-04-2016, 02:03 PM
Mine is not set up yet but Monitor on wall and keyboard mouse just below on swinging shelf or a 14" CRT tv bracket in a former life with a piece of MDF attached swings all ways including back to wall up out of way of chips. I also have the Mill sitting in a 700x700x7mm plastic garland tray from amazon catches lots of chips and fluis if necessary come in all different sizes extremely useful in workshop.
http://www.amazon.co.uk/Garland-2251-GARLAND-SQUARE-GARDEN/dp/B000VPDIZ8?ie=UTF8&psc=1&redirect=true&ref_=oh_aui_detailpage_o05_s00

Davek0974
17-04-2016, 03:32 PM
As a move in the right direction, i have fitted some bracketry and mounted the monitor up high out of the chip path, the brackets stem from the main table frame which is 44x44 structural aluminium, makes it easy to bolt bits on ;)

I also did a facing cut on the bed, here's a video of a bit of it...
https://youtu.be/PSkSn_s8xF8

It was with a 12mm indexable carbide tool at 21000 rpm and 2300mm/min feed, DOC was 0.15mm, just enough to get a cut off the whole face.

The results show the head is a tiny bit off-tram but until i get a decent setup for adjusting it I think it best left where it is, using a DTI it seems the slight ripples made by the tool are about 0.01mm high at the peak,not bad i think as the head was just as i bolted it on!

All things being equal, the results from now on should be 'as good as it gets' for a while at least.

Davek0974
02-05-2016, 07:47 PM
Still running good, much better in fact after doing the facing cut on the bed - i think this should be the first job on any machine as it makes such a difference.

Now have Vectric software which seems pretty good. Does anyone here use it know if there is a way to enter g-code snippets into the job process list??

Things like selecting G5x Offset or adding a pause, message etc ??

routercnc
02-05-2016, 08:02 PM
Don't know about inserting g-code using Vectric directly, but you can read the .txt gcode files it creates using a text editor such as 'notepad' and add the lines manually. Or you can load the code into Mach3, then there is a code editing button which opens a text editor which you can then edit.

Davek0974
02-05-2016, 08:08 PM
Yeah thanks, I knew about the manual edits but I am sort of side-stepping from SheetCam to Vectric for the mill stuff and sheetcam can do code inserts easily, saves a lot of messing around when running and modifying a file repeatedly.

Ger21
02-05-2016, 09:00 PM
You can edit the post.

Look in the post processor manual. There's a variable called "file notes" that you can add.
In Cut 2D or V Carve Pro, go to Edit > Notes and put your G5x there.
Then the notes will be inserted in the g-code wherever you put the "file notes".

Davek0974
02-05-2016, 09:49 PM
OOH, nice ;)

Didn't notice the post manual before.

I see there is possibly a more useful one called [TOOL_NOTES] that goes with each tool used, the post wraps the message in brackets which are ignored by Mach so it will need some editing which will then render the [TOOL_NOTES] feature useless for tool notes but hay-ho you can't have it all I guess ;)

Just insert the tool_notes var into the tool change part of the post, as i want add a macro call to go to park position and then a pause to remind me to change hold-down clamps etc before changing the tool and continuing.

Ger21
03-05-2016, 01:45 AM
I see there is possibly a more useful one called [TOOL_NOTES]

That depends on what you want to do.
For adding a G5x, I think the file notes are a better choice.

For the park position, add the M883 at the start of your tool change section in the post, followed by your pause.

Davek0974
03-05-2016, 07:16 AM
Its more complex as usual :)

The park position is only needed on a couple of jobs which need to be part machined then the clamping moved around and the tool changed then the finish cuts made.

There are three options i see tool_notes, toolpath_notes and file_notes - all look useful.
The G5x only needs calling at the start of one particular file.

:)

A_Camera
16-05-2016, 08:57 AM
Sorry typo
3mm high and ~12mm long
Careful filing and sanding then scouring pad gives a reasonable finish. If you want a mirror finish with no sign of tabs then you are back to fixing the part down in the middle using any holes that are available instead of using tabs.

On occasion I've also put the raw tabbed part in a vice edge up and used the machine to skim it down 0.05mm at a time and remove the last but if the tab. You can get a very good finish but you ideally need a parallel edge on the lower side to reference to sitting in the vice. But this takes time and is best for simple shapes.

Why not using the "onion skin" method Jazz mentioned earlier? I think that a 0.1mm onion skin would give the same holding strength (probably even better) as a 3 x 12mm would, assuming you have 4 tabs with that size, converting that to onion skin, you can have a total circumference of 1440mm if you have a skin of 0.1mm. In my opinion it is easier to clean off the edges if only 0.1mm must be cleaned than if 4 times 3 x 12mm must be cleaned.

Davek0974
16-05-2016, 07:53 PM
As some may have read, I am converting my Bridgeport mill to CNC, the idea is to attache the high speed spindle to it to make a dual purpose machine.

Seems I have a couple of options here - mount the spindle motor to the main mill quill or make a new Z axis complete and mount that to the head of the Bridgeport.

Mounting the spindle to the quill is easiest - a simple clamp block would do it...
18475
The larger circle is the mill quill or Z axis (around 100mm dia), smaller is the 24k spindle (80mm dia), looking down from above. The distance between the two is 50mm and the clamp could be machined from 30-40mm thick aluminium or similar.

Would it work though??
Your thoughts...

Second option is far more involved and needs a mounting bracket and complete Z axis making to take the 24k spindle, this assembly would mount on the rear of the swivel ram (at the back in this picture)...
18476

Would be harder to make but still do-able but if the first idea worked the much time and cash will be saved ;)

Thoughts??

lucan07
16-05-2016, 08:16 PM
Why do you want 24k on the mill surely you would be better having some lower end torque and going for maybe 6-10k, 6k bottom end seems to high for a mill, I may be completely wrong as a complete noob but I would have thought you are losing more than your gaining with a 24k with bottom end around 6k.

JAZZCNC
16-05-2016, 08:27 PM
I'd come of the quill to save grief. Chances are you'll only use small tooling anyway so no great stress.

Davek0974
16-05-2016, 08:43 PM
Why do you want 24k on the mill surely you would be better having some lower end torque and going for maybe 6-10k, 6k bottom end seems to high for a mill, I may be completely wrong as a complete noob but I would have thought you are losing more than your gaining with a 24k with bottom end around 6k.

It's all about flexibility - the mill itself has 2Hp and 50-3000rpm range - no good for small cutters or engraving, great for hogging the crap out of steel etc with large tooling. The spindle has the speed for small cutters and engraving but no good for big tooling or steel work. The Base machine is simply a very heavy X/Y table - 300mm in Y and 1000mm in X - way bigger than my mini-mill.


I'd come of the quill to save grief. Chances are you'll only use small tooling anyway so no great stress.

That's my view too, I have 125mm of Z axis movement and losing 30-40mm for the clamp won't hurt as there is also a manual 300mm of table up/down - no engraving spindle is going to be diving more than 80mm into the work so travel seems adequate even allowing for clearance plane above clamps etc.

This is also the easy option to test out - only wastes a block of aluminium if it fails, my point of weakness would likely be vibration causing chatter marks, but time will tell here.

lucan07
16-05-2016, 08:57 PM
It's all about flexibility - the mill itself has 2Hp and 50-3000rpm range - no good for small cutters or engraving, great for hogging the crap out of steel etc with large tooling. The spindle has the speed for small cutters and engraving but no good for big tooling or steel work. The Base machine is simply a very heavy X/Y table - 300mm in Y and 1000mm in X - way bigger than my mini-mill.

If its about flexibility then why not keep the grunt and mount a spindle to one side might have to extend arm on right past the 24k spindle but looking at it should be possible, the you would probably still have 800x300 travel on the 24k and the ability to hog the crap out of steel when needed. I would be a fantastic base for a router for engraving and using small endmills but severely limited in the type of work it was designed to do

Davek0974
16-05-2016, 09:07 PM
That is exactly my plan, should have explained better ;)

The 24k spindle is not going be full-time mounted, its an option and will be pulled off when not needed.

Due to the way the head swivels on the BP I can probably maintain near full X travel if needed just by moving the ram to the left when the spindle is in use, its a very flexible machine - that's why i like it so much.

JAZZCNC
16-05-2016, 09:07 PM
If its about flexibility then why not keep the grunt and mount a spindle to one side

Maybe you need to read again because that's exactly what Dave's talking about doing.!!

lucan07
16-05-2016, 09:15 PM
Obviously I missed something, somewhere in the posts.

Davek0974
17-05-2016, 08:47 PM
The clamp block for holding the spindle to the mill, better made out of one big lump or two plates maybe 12mm thick spaced apart 10mm or so?

Lee Roberts
17-05-2016, 09:49 PM
The clamp block for holding the spindle to the mill, better made out of one big lump or two plates maybe 12mm thick spaced apart 10mm or so?
My choice would be a single lump or to space them out more if it's for a typical water cooled spindle, 12's a bit thin in my book.

.Me

Davek0974
17-05-2016, 09:56 PM
Just realised they would need to be firmly fixed to each other or it would allow twist. Single block it is ;)

Davek0974
17-05-2016, 09:59 PM
Will be using two Mach3 profiles. Only one spindle will be in use at any time.

Looking for ways to switch all the control lines needed -

Vfd supplies
vfd control and fault lines
vfd speed lines
limit switches for Z axis in two positions
homing for z axis in two positions
cooling pump for 24k spindle
probably others....

The programming for the CSMIO plugin I gather will need to be the same for both profiles?

Davek0974
04-07-2016, 07:43 PM
Odd programming?

I am cutting some plate for parts on my Bridgeport conversion project, had some good success and a couple of oddities. The most annoying one is my motor VFD has shut down twice now with an error that shows as short-circuit on motor phases, each time i reset and it carried on ok, there was a month between faults - the annoying part is i don't have the fault relay in my e-stop loop (yet) so the motor quits and the motion caries on - snap goes another 8 tool :(

The rest of my issues are experience, or lack of, related so in the end i worked them out, but I'm getting pretty good at re-homing and starting over with modified code ;)

Davek0974
11-07-2016, 07:30 PM
7000rpm on a 8mm 2-flute cutter too much?

Just been trying to carve a lump of 18mm thick ally for my Bridgeport conversion, using a 2-flute 8mm HssCo tool at 7000rpm, 900mm/min and 1.6mm DOC

All the features went without hitch, the perimeter decided to bog-down after getting about 9mm deep and stalled the axis.

I have a feeling the height of the wall blocked the coolant/air and allowed the tip to build-up. I need to fit two coolant jets i think at 90deg to each other.

I have re-cammed the profile starting from 8mm down and increased rpm to 8000 and reduced step-over a little.

Will see what happens tomorrow.

routercnc
12-07-2016, 06:52 AM
Hi Dave,

That used to happen to me a lot. Slot milling over 8mm risks poor chip evacuation and clogging of the tool. I've seen people machine the outside material completely away (i.e. an outer pocket to leave the central island, not a perimeter slot). But then you need to be able to hold the part in the middle which isn't always possible.

Another option is to use something like adaptive machining to mill a larger width slot than the tool.

I tend to reduce the DOC when over 8mm into a slot and that works OK. I vacuum out the slot on every pass and give a quick spray of WD40.

Davek0974
12-07-2016, 07:23 AM
Adaptive does look good but none of the CAM software i have can do it.

I tend to pocket the part out, leaving tabs etc to hold it, on the 8mm tool i used a 12mm pocket so two passes, but when the tip is deep in the pocket the air/coolant cant reach it and i was not paying enough attention i guess.

I'll see if i can rescue the part with the modified paths and some extra air blast.

Davek0974
12-07-2016, 06:56 PM
Beginning to think i may never get this part cut :(

I increased the speed to 9000rpm, and dropped the feed-rate a little as well as reducing the DOC a little.

Good news was that it picked up the position ok.

It made it about three passes then bogged down again, this time i hit the stop button pretty quick.

Restarted and after a couple of passes cutting air, the motor turns off!
No message on the VFD or screen.

I gave up at this point and went in for dinner.

So, why would the motor turn off if Mach did not know and there was no fault on the VFD?

Davek0974
13-07-2016, 06:07 PM
No idea why the motor turned off, it run ok tonight. Even managed to get the part finished.

Reduced DOC to 1mm, feed rate to 800mm/min and rpm up to 9000.

I think the issues may the cutter itself, not being designed for aluminium, just a standard two-flute slot drill.

Now i need to flip it over, align to the axes and find an accurate way of picking up the x&Y datums.