Questions on using a moving gantry style mini-mill...

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....

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.

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.

Quote:

---

Originally Posted by Davek0974

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.!!!

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...

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.

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 ;)

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:
Attachment 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?

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.

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.

Quote:

---

Originally Posted by lucan07

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;)

Quote:

---

Originally Posted by Ger21

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.

Quote:

---

Originally Posted by Davek0974

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 :)

Quote:

---

Originally Posted by CharlieRam

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 ;)

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.

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.

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.

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

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 :(

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 :-)

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.

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.

Quote:

---

Originally Posted by Ger21

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 :)

Glad it helped, If you drill the holes first, then do the pockets and outer profile, m00 etc. would that reduce tool changes?

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........

Already planning Version 2.0?

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 £££££

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???

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

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 ;)

Attachment 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.

IIRC the timer gets reset every time you press cycle start.

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 . . .

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.

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 ;)

Attachment 18214

Attachment 18215

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....

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...ilpage_o05_s00

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.

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 ??

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.