-
1 Attachment(s)
Questions on using a moving gantry style mini-mill...
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;)
Attachment 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
-
Re: Questions on using a moving gantry style mini-mill...
How are you going to do the 90' corners?
-
Re: Questions on using a moving gantry style mini-mill...
Quote:
Originally Posted by
Clive S
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.
-
Re: Questions on using a moving gantry style mini-mill...
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
-
Re: Questions on using a moving gantry style mini-mill...
Quote:
Originally Posted by
routercnc
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
-
Re: Questions on using a moving gantry style mini-mill...
#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.
-
Re: Questions on using a moving gantry style mini-mill...
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
-
Re: Questions on using a moving gantry style mini-mill...
Quote:
Originally Posted by
Davek0974
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.
Quote:
Originally Posted by
Davek0974
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.?
-
Re: Questions on using a moving gantry style mini-mill...
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?
-
Re: Questions on using a moving gantry style mini-mill...
Quote:
Originally Posted by
Davek0974
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.
Quote:
Originally Posted by
Davek0974
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.
Quote:
Originally Posted by
Davek0974
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.
-
Re: Questions on using a moving gantry style mini-mill...
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 ;)
-
Re: Questions on using a moving gantry style mini-mill...
Quote:
Originally Posted by
Davek0974
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.
-
Re: Questions on using a moving gantry style mini-mill...
-
Re: Questions on using a moving gantry style mini-mill...
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??
-
Re: Questions on using a moving gantry style mini-mill...
Rough cut the 3 slots in multiple passes before making your full depth perimeter cut.
-
Re: Questions on using a moving gantry style mini-mill...
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?
-
Re: Questions on using a moving gantry style mini-mill...
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.
-
Re: Questions on using a moving gantry style mini-mill...
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.
-
Re: Questions on using a moving gantry style mini-mill...
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.
-
Re: Questions on using a moving gantry style mini-mill...
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.
-
Re: Questions on using a moving gantry style mini-mill...
Its my brain thats limited i think ;)
Messing with various ideas now, as you said, thinking differently to get the job done that matters.
-
Re: Questions on using a moving gantry style mini-mill...
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 ;)
-
Re: Questions on using a moving gantry style mini-mill...
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 :)
-
Re: Questions on using a moving gantry style mini-mill...
Quote:
Originally Posted by
Davek0974
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.
Quote:
Originally Posted by
Davek0974
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.?
-
Re: Questions on using a moving gantry style mini-mill...
Thanks Jazz, all noted.
Dave
-
Re: Questions on using a moving gantry style mini-mill...
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 ?
:)
-
Re: Questions on using a moving gantry style mini-mill...
Sorted :)
Use Job Options -> ToolChange -> "run code before tool change" box and enter
G53 G1 Z0 F1500
or
G53 G0 Z0
Works perfectly
-
Re: Questions on using a moving gantry style mini-mill...
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?
-
Re: Questions on using a moving gantry style mini-mill...
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.?
-
Re: Questions on using a moving gantry style mini-mill...
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 :)
-
Re: Questions on using a moving gantry style mini-mill...
When running Mach3 without the parallel port driver installed, a lot of things don't work correctly.
-
Re: Questions on using a moving gantry style mini-mill...
That explains it then, thanks.
-
Re: Questions on using a moving gantry style mini-mill...
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.
-
Re: Questions on using a moving gantry style mini-mill...
Done, looks very nice indeed.
Do you get commission ;)
Thanks
-
Re: Questions on using a moving gantry style mini-mill...
Quote:
Originally Posted by
Davek0974
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:
-
Re: Questions on using a moving gantry style mini-mill...
Some good people on here, no two ways about it :fat:
-
Re: Questions on using a moving gantry style mini-mill...
Quote:
Originally Posted by
JAZZCNC
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 ;)
-
Re: Questions on using a moving gantry style mini-mill...
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.
-
Re: Questions on using a moving gantry style mini-mill...
Turn off Auto screen enlarge and they won't be fuzzy. I use an old 15" monitor myself.
-
Re: Questions on using a moving gantry style mini-mill...
Arrived last night, looks money well spent, nice one.:thumsup:
Day off today, out in the shop, get the thing going :)