Machsupport Forum
Mach Discussion => Mach4 General Discussion => Topic started by: propstuff on May 20, 2021, 12:54:44 AM
-
Hi.
SheetCam 7.0.7, Mach4 Plasma Post
Mach4 4.2.0.3233
ESS 1.0.1.193
When using the above set up and Mach comes to make a rapid between cuts, the Z is not retracting to it's safe height prior to the X/Y travel. instead it is progressively reaching it's Z height in the same sort of way that the X and Y axis do over the full extent of the move. This is causing problems.
When I run a simulation in Sheetcam, the Z moves to it's correct height before the X and Y move at all (as expected), but not when I actually run it in Mach4
When I run the machine as a router with the same setup, but using a Mill/ Router post this doesn't happen and the spindle retracts prior to rapids as expected.
If I insert a line in the code "Z##" after the M05 line and prior to the G00 Z### Y### line it behaves as expected, but I don't want to have to manually do this obviously
Can anyone tell me where and how in Mach/ESS I need to set this up??
TIA,
Nicholas
-
**Bump**
Noone from Artsoft can help with this?
I've attached a copy of the Profile if that helps.
At the moment I'm cutting a few simple parts at a time from each sheet, and it's a nuisance editing the code by hand, but when I come to doing multiples of complicated parts it's going to be unworkable...
Hoping someone can help (?)
-
Hi Propstuff,
This forum is really just for members to communicate / discuss issues and, of course, help others if they can. Although this thread is monitored by Goomba, on behalf of Artsoft / NFS, he does not always reply to every post.
If you need a problem to be looked at by Artsoft / NFS specifically then you need to contact them directly by way of their Help Desk ; https://www.machsupport.com/support/
Tweakie.
-
Hi propstuff,
That almost sounds more a post processor issue than a Mach4 issue. If you can fix the issue by adding a line of gcode. the posts should be able to do that!!
That said, support is going to want you on a WAY newer version (4612 at least) and if you truly have an ESS and not a USB Smoothstepper, USS, you'll be nudged to a new plugin, too. ESS Mach4 plugins don't even use that numbering convention now.
You might rename your Mach4Hobby folder, install Mach4 new, and copy you plugins, profiles, screensets, macros, whatever, into the new version so you can fall back by simply renaming directories, too.
Tom
-
Thanks for the replies.
Good of you to take the time.
I've downloaded the updates and I'll install them when I'm clear of the current business.
In the meantime, this is a little chunk of the code Sheetcam is writing (from one cut to the next)
.......
N0100 Z0.0000 M03
N0110 G02 X98.2146 Y1181.7854 I1.7854 J-1.7854 F5000.0
N0120 M05
N0130 G00 X1301.7854 Z20.0000
N0140 Z0.0000 M03
.......
At line 130, SheetCam simulates this as the Z move completing before the X move starts.
Is this what you would expect Mach4 to do from the way this is written?
cheers
Nicholas.
-
Ok, I've installed the latest versions (and trying to work through the "A axis etc Go To Work Zero button doesn't work" bug, but aside from that...)
I went back through some old router files and also ran the SheetCam file with different Post options (and learnt a bit more about Gcode in the process)
Where the head is retracting to a safe Z prior to XY moves, SheetCam is writing a G00 Z## line prior to the XY line just as I have been manually adding.
So; even though Sheetcam's simulation shows the Z move completing prior to the XY, when you have a line of G00 X## Y## Z##, all 3 axis moving progressively to the point is normal expected behaviour.
Is this correct?
-
Thanks for the replies.
Good of you to take the time.
I've downloaded the updates and I'll install them when I'm clear of the current business.
In the meantime, this is a little chunk of the code Sheetcam is writing (from one cut to the next)
.......
N0100 Z0.0000 M03
N0110 G02 X98.2146 Y1181.7854 I1.7854 J-1.7854 F5000.0
N0120 M05
N0130 G00 X1301.7854 Z20.0000
N0140 Z0.0000 M03
.......
At line 130, SheetCam simulates this as the Z move completing before the X move starts.
Is this what you would expect Mach4 to do from the way this is written?
cheers
Nicholas.
Far from the expert, I'd say NO, X and Z will move simultaneously. Try it in air, then add line 125 G0 Z20.0000 and see what you get.
-
put them on separate lines (blocks )
then they will move independently
for example a90 x50. will produce a quarter turn helix
but
a90
x50
will rotate a then move x
that's my 2 cents
-
So, the conclusion is:
Mach is behaving as expected.
SheetCam is writing code in the Plasma Post where the Z does not retract first at rapids.
SheetCam is writing code in the Router Post that does retract the Z first. (as necessary)
Something odd is going on in SheetCam's Simulation where it is showing the Z retracting before the XY rapids.
Thanks again for the input.
Nicholas.
-
Your conclusions look good with the exception that I think the sheetcam simulation is correct. That is what is is supposed to do. However, what sheetcam is writing out for G code is NOT correct, at least for the plasma post. So I would most definitely take a look at the plasma post processor first. The task of a post processor is to make G code (for s specific machine) that does EXACTLY what the simulation does.
Steve
-
Thanks for the thoughts Steve. I have limited experience.
I note that SheetCam has a Post option something along the lines of "Mach4 Plasma no Z" or something like that, as well as the "Mach4 Plasma" option.
Generally, would a plasma post be expected to retract between rapids?
-
Yes, if the part being cut has many cuts or obstacles instead of one long single cut. Basically, the machine SHOULD operate as per the simulation in sheetcam.
Steve
-
Thanks again Steve.
I'll head over to SheetCam and see what I can find out there.
Nicholas.