Project 1 from EmptyNester. Category: Custom Shop Tools - CNC Table

Here is a basic square with 0.020" offset for a 0.040" kerf with comments for each line. It's set nice and slow so you can follow it easily as it runs. I left out the corner arcs and leadin/outs so it's super easy to follow.

N100 G20 (Units: Inches)
N110 G53 G90 G40 (Setup no offsets, absolute, no comp)
N120 M06 T1 F20 (Plasma - outside profile, 20 ipm)
N130 G00 Z2.500 (Rapid Z to safe height 2.5")
N140 X2.02 Y-0.02 (Rapid to start point)
N150 Z0.500 (Rapid to pierce height .5")
N160 M03 (Start torch)
N170 G04 P2. (2 second pierce pause)
N180 G01 Z0.100 (Feed to cut height .1")
N190 X-.02 (First side)
N200 Y2.02 (Next)
N210 X2.02 (Next)
N220 Y-0.020 (Next)
N230 M05 (Stop torch)
N240 G04 P1. (Pause for post flow 1 second)
N250 G00 Z2.500 (Rapid Z to safe height)
N260 X0.000 Y0.000 (Rapid to home)
N270 M30 (End program)

Rambozo - thanks. I ran that and it went as expected.

I took one of the odd ones I've generated and stepped through them to identify the commands. I deleted the circles. It seemed to work okay.

I'll spare the details, but I tried lots of different things and was always getting the conincentric circles in the Mach driver. I run Mach on a PC in the garage and have my drawing program and SheetCam upstairs. To try to save time debugging, I installed mach on the upstairs PC. Everything looks fine. The same file loaded on the table's Mach driver is messed up.

At this point, I think I have a very hosed installation/configuration on the table's Mach driver.

There are some options in the configuration for arcs. Every control is different, and Mach can be configured to behave in a few different ways. For instance I use an Anilam control that uses absolute coordinates for the centerpoint if the endpoint is absolute, while the standard for Mach and some other controls is that center points are incremental offsets, even when you are in absolute mode. In fact I had to switch my backplot program to get a proper display for your code. Just like some controls can't do a full circle with one arc command, some are limited to 90° and some to 180° so you have to break the circle into multiple arcs.

Here is a sample with an incremental centerpoint arc.
N100 G20
N110 G53 G90 G40
N120 M06 T1 F20
N130 G00 Z2.500
N140 X1. Y1.
N150 Z0.500
N160 M03
N170 G04 P.5
N180 G01 Z0.100
N190 Y3.
N200 G2 X3.Y1.I0.J-2.
N210 G1 X1.
N220 M05
N230 G04 P1.
N240 G00 Z2.500
N250 X0.000 Y0.000
N260 M30

And here is one with absolute.
N100 G20
N110 G53 G90 G40
N120 M06 T1 F20
N130 G00 Z2.500
N140 X1. Y1.
N150 Z0.500
N160 M03
N170 G04 P.5
N180 G01 Z0.100
N190 Y3.
N200 G2 X3.Y1.I1.J1.
N210 G1 X1.
N220 M05
N230 G04 P1.
N240 G00 Z2.500
N250 X0.000 Y0.000
N260 M30

And finally here is an example where all the X Y moves are in incremental by switching the mode with a G91.

N100 G20
N110 G53 G90 G40
N120 M06 T1 F20
N130 G00 Z2.500
N140 X1. Y1.
N150 Z0.500
N160 M03
N170 G04 P.5
N180 G01 Z0.100
N190 G91
N200 Y2.
N210 G2 X2.Y-2.I0.J-2.
N220 G1 X-2.
N230 M05
N240 G90
N250 G04 P1.
N260 G00 Z2.500
N270 X0.000 Y0.000
N280 M30

I reinstalled Mach and I was still having problems.

After looking through the Mach support forums, I found out that this is a common problem. The "IJ Mode" has to be set to "Incremental". That took care of it.

I'm anxious to give it a try, but may wait until the weekend so I have time to play.

You can have the IJ in absolute, you just need to tell SheetCAM to be that way, too. I actually like to keep everything in absolute or everything in incremental depending on G90 or G91. That mixed mode is a pain to work with, but I think Fanuc decided that was going to be their standard and everyone copied them.
There are also option where you can use radius for arcs with the R command. Here is a better explanation than I can give all about arcs.

http://www.cnccookbook.com/CCCNCGCodeArcsG02G03.htm

There are even some options in CAM programs to not use arcs at all. The CAM program will create all the arcs as a series of very small straight line moves. The programs get huge, but some controls can actually run them faster than having the control compute the arcs, especially with other options running like cutter comp, or rotation/scaling/offset commands running.

Did the first cut. After all the dry runs, it worked out pretty good.

I cut a square but had a problem that the arc went off at the corners. I have to try to figure out why that happened. I'm not sure if it's a configuration issue for Mach or Sheetcam (I had "loop corners" set to triangle - my primary suspect) or if a noise issue with my Arduino THC that controls the torch on and arc good.

Top of cut:
Attachment 8161

Bottom of cut:
Attachment 8162

I'm sure it will take a while to figure out optimum settings.

Did you fix SheetCAM so the corners are not still at 200 ipm?

Beats me.

I thought I was cutting at 10 ipm, which seemed slow.

I'm not sure where the speed is in the G-code:

N0010 (Post processor: MP1000-THC.scpost)
N0020 (Date: 10/10/2012)
N0030 G20 (Units: Inches)
N0040 G53 G90 G40
N0050 F1
N0060 (Part: SquareStar)
N0070 (Process: Set variable switchoffset = 0.2)
N0080 (Process: Outside Offset, Layer 2, T1: Plasma - outside profile)
N0090 M06 T1 F10 (Plasma - outside profile)
N0100 G00 Z2.0000
N0110 X2.3082 Y-0.1319
N0120 Z0.5000
N0130 G28.1 Z0.12
N0140 G92 Z0.0
N0150 G00 Z0.2000
N0160 G92 Z0.0
N0170 G00 Z0.5000
N0180 M03
N0190 G04 P0.3
N0200 G01 Z0.0800 F20.0
N0210 G02 X2.2058 Y-0.0295 I0.0000 J0.1024 F10.0
N0220 G01 Y0.0000
N0230 Y2.0075
N0240 Y2.1404
N0250 X2.3091 Y2.0371
N0260 X2.1762
N0270 X0.0000
N0280 X-0.1329
N0290 X-0.0295 Y2.1404
N0300 Y2.0075
N0310 Y0.0000
N0320 Y-0.1329
N0330 X-0.1329 Y-0.0295
N0340 X0.0000
N0350 X2.1762
N0360 X2.2058
N0370 G02 X2.3082 Y-0.1319 I0.0000 J-0.1024
N0380 M05
N0390 G04 P0.5
N0400 G00 Z2.0000
N0410 X0.0000 Y0.0000
N0420 M05 M30

N0210 G02 X2.2058 Y-0.0295 I0.0000 J0.1024 F10.0

The feedrate is the "F10"

Try changing the 10 to a 20 or 30 and rerun the program exactly the same otherwise and you will see the difference.

You mention "triangles" for the corners. If you look at the plan view, you can see the triangles formed at the corners. Basically the toolpath runs past the edge by say 3/16", then turns and moves across the hypotenuse of the triangle, then proceeds to cut the next side. I doubt this has anything to due with the arc going out.

Quote:

---

Originally Posted by EmptyNester

Beats me.

I thought I was cutting at 10 ipm, which seemed slow.

I'm not sure where the speed is in the G-code:

N0010 (Post processor: MP1000-THC.scpost)
N0020 (Date: 10/10/2012)
N0030 G20 (Units: Inches)
N0040 G53 G90 G40
N0050 F1
N0060 (Part: SquareStar)
N0070 (Process: Set variable switchoffset = 0.2)
N0080 (Process: Outside Offset, Layer 2, T1: Plasma - outside profile)
N0090 M06 T1 F10 (Plasma - outside profile)
N0100 G00 Z2.0000
N0110 X2.3082 Y-0.1319
N0120 Z0.5000
N0130 G28.1 Z0.12
N0140 G92 Z0.0
N0150 G00 Z0.2000
N0160 G92 Z0.0
N0170 G00 Z0.5000
N0180 M03
N0190 G04 P0.3
N0200 G01 Z0.0800 F20.0
N0210 G02 X2.2058 Y-0.0295 I0.0000 J0.1024 F10.0
N0220 G01 Y0.0000
N0230 Y2.0075
N0240 Y2.1404
N0250 X2.3091 Y2.0371
N0260 X2.1762
N0270 X0.0000
N0280 X-0.1329
N0290 X-0.0295 Y2.1404
N0300 Y2.0075
N0310 Y0.0000
N0320 Y-0.1329
N0330 X-0.1329 Y-0.0295
N0340 X0.0000
N0350 X2.1762
N0360 X2.2058
N0370 G02 X2.3082 Y-0.1319 I0.0000 J-0.1024
N0380 M05
N0390 G04 P0.5
N0400 G00 Z2.0000
N0410 X0.0000 Y0.0000
N0420 M05 M30

---

Looks like the Z move from pierce to cut height is at 20 then everything else is at 10. F stands for Feedrate and stays active until a change. It can be appended to a motion command but takes effect before that move. I bet 10 is kinda slow for that cut.

Thanks for the feedback guys.

I found a reference so I could start learning G-code. It looks like the G-code never turned off the torch, so I'm guessing it was due to the noise on the interface from the motors when they cut the corners and doubled speed and made quick direction changes.

I didn't put a ferrite on the BOB -> THC cable yet. That's probably the first step. If that doesn't do it, I guess I can delay the torch off in software (probably start with 250 ms and take it up from there). I'd prefer to address the noise, but I think I could end up cutting/wasting a lot of steel getting scope captures to figure out what's going on.

I think that the cut rate was way too slow. I had been trying to find a good chart to give me a starting point for cutting speeds and amperage settings based on thickness. I finally found a decent starting point on Eagle Plasma's web page:
http://eagleplasma.com/4x4system.html

It recommends 240 ipm @ 30 amps for 16 ga. I cut the 18 ga at 10 ipm @ 35 amps.

I am really confused.

I can't seem to figure out how to configure Mach to use the Arc Okay signal. The signal is working, but I can't find anything in the doc or online about how you actually configure Mach to use Arc Okay.

Anybody have any ideas?

I'm still trying to figure out why the torch cuts out while cutting. I don't hear the relay click off, or see the Arduino say the torch was turned off. It could be so fast that I don't see and hear it. I'll have to watch voltages. But, I really think its a configuration issue.

I feel like Mach and Sheetcam are each a "universal mounting bracket" from different companies that need to work together. But, you just can't figure out how.

Thanks.

I would think that ARC GOOD would have to be configured in that custom G28.1 routine for THC.

Since your corners end up a basically a big hole, maybe because you are going too slow the arc just cuts out from the gap, and not from any signal. I would think you would be able to tell from the relay and status indicators that the plasma has been stopped by a signal. Maybe that was part of the reason for the high speed in the corners? Now that you have your arcs fixed, you can go back to corner loops and maybe make them a little larger so there is some metal under the plasma jet and not a hole from the other part of the loop. All of these are more SheetCAM issues. I think you have Mach doing just what it is told to do.

Is Mach honoring your pierce delays?
This post seems to indicate that with the THC set, the arc ok signal is being used and the delay might be expected from the THC which is probably not the best system. You can modify a macro to fix this, but i believe it has been reported as a Mach bug.

http://www.machsupport.com/forum/ind...?topic=17435.0

I believe the proper path should be:

Move to pierce height
Start arc
Test for Arc ok and wait for it, with a timeout after a long time and end program with an error.
Start pierce delay
End pierce delay
Move to cut height
Start X-Y motion

It looks like you have to make some adjustments to get this to work.
It might be to be compatible with THC's that do their own pierce delay internally. Maybe research this a little to see if it's something you want to add. I think I would rather have that added by the CAM program. There are pros and cons to each method.

To make things easier to debug, maybe you would be better suited to just cut a simple square with no change in the corners at all. Or maybe a circle.

You could just manually program a square without any offset or any fancy stuff at all, just make the torch pierce then move in a square then stop.

Quote:

---

Originally Posted by sportbike

To make things easier to debug, maybe you would be better suited to just cut a simple square with no change in the corners at all. Or maybe a circle.

You could just manually program a square without any offset or any fancy stuff at all, just make the torch pierce then move in a square then stop.

---

Personally I would make it real simple and program a straight line with a an increasing feedrate to learn what speed makes the best cut for my combination of torch, amps, and material.

Something simple like starting from X0 Y0:

G1 X1.0 F20
G1 X2.0 F30
G1 X3.0 F40
G1 X4.0 F50
G1 X6.0 F60

Run that across a 6" piece of your sample material and see what it looks like. If it completes the cut, crank up the speeds and run it again. Then you will see what speed you need to make the cleanest cut and where it breaks down both above and below. That will give you your speed envelope. You can do finer increments if you need to break it down further, once you have the ballpark numbers. The correct feedrate will allow your cam package to do the correct compensations for curves and such. You can also program a series of pierce delays to figure out how long to make that, just a series of holes spaced apart. Make each one shorter until it fails to pierce. I'm sure you want a little buffer there, but again it would give you some ballpark figures for your combination.

Quote:

---

Originally Posted by Rambozo

Personally I would make it real simple and program a straight line with a an increasing feedrate to learn what speed makes the best cut for my combination of torch, amps, and material.

Something simple like starting from X0 Y0:

G1 X1.0 F20
G1 X2.0 F30
G1 X3.0 F40
G1 X4.0 F50
G1 X6.0 F60

Run that across a 6" piece of your sample material and see what it looks like. If it completes the cut, crank up the speeds and run it again. Then you will see what speed you need to make the cleanest cut and where it breaks down both above and below. That will give you your speed envelope. You can do finer increments if you need to break it down further, once you have the ballpark numbers. The correct feedrate will allow your cam package to do the correct compensations for curves and such. You can also program a series of pierce delays to figure out how long to make that, just a series of holes spaced apart. Make each one shorter until it fails to pierce. I'm sure you want a little buffer there, but again it would give you some ballpark figures for your combination.

---

That's a damn good idea Ram. Once a rough idea of speed is figured out, straight lines with variable THC voltage settings could be done to dial height in as well.

Probably could get a pretty good idea on speeds and feeds from using two or three material thicknesses and spending about to minutes on each one, then interpolating the results for other thicknesses.

Because of all the problems, I stepped back and spent the day watching Mach and SheetCam videos and reading the manuals and just doing some testing to learn a little more about how the plasma cutter works.

I hadn't used the plasma enough to realize that I'd loose arc at about 1/4" above the metal. (I had always been dragging or using the standoff when cutting.)

At a minimum, some of the issues I found were:

• pierce and cutting height too high (causing the arc to go out)

• not really understanding Mach's coordinate systems and how to use it

• Spindle delay was on which added to pierce delay

After reinstalling Mach and Sheetcam, I was able to successfully cut a 1" circle. I still have to tune my settings (Ram - your straight line method with different speeds is a great idea).

Mach seems to have very little documentation on using plasma. It was only a side comment in one of the videos that said "THC On" actually is the "Arc Good" input. So, I've configured that - but it doesn't seem to stop the motors if the arc goes off. Does the "THC" feature have to be turned on?

Given how such a small gap can cause loss of arc - I can see why it may not be practical to cut thin metal without a THC.

I tried my first cut of a shape other than a circle. I made a name plate for my wife that I could mount in a wood base.

Everything worked great, but the cut wasn't very clean. I'm guessing that I had the torch too high. Any thoughts would be appreciated.

Attachment 8354