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

[Davek0974]

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]

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]

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]

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

[Davek0974]

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]

Already planning Version 2.0?

[Davek0974]

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]

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]

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]

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 ;)



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.