Losing steps and ruining parts, help me, you'll be my hero

Hey guys, new-ish cnc'er, have a new PCNC 1100 with the Tormach controller, generating gcode with HSMxpress and the 'Tormach_NexGenCAM_110911.cps' post processor. I'm having a major issue with Z height repeatability and I think it has to do with Mach3 and helixing and ramping. I make lots of pockets and I'm wondering how anybody else uses their Tormach to pocket and expect it to perform as commanded.

Ok, so I'll CAM my part in HSMxpress, the gcode is correct (dealing only with Z axis right now, the others are phucked the same way but not as much, if we can fix Z, I bet it fixes it all). There's a simple facing operation followed by two pocket operations on the same center, different diameter, not big deal. If I helix into the stock at 350mm/min (~15ipm) using small or large radius helix, I lose Z position by 2.5mm. I'm cutting down 2mm (0.080") at a time with a 2 degree ramp. Not every helix operation loses steps.

So I switched to a zig-zag operation instead of a helix, using only 2 axes at a time. I made two zig-zag/clear passes and lost Z again by 2.5mm; I checked the Z height with the tool on the workpiece just prior to pushing cycle start and it was fine, so Mach made two zig-zag pocket moves, picked up and moved to cut a profile and was 2.5mm too deep. So I'll run a test with a dial indicator of the table,

This is killing me, I don't trust Mach and I can't cut parts. How is this possible?

How about another approach for you awesome forum gurus: Is anybody using HSMxpress, the Tormach controller and Mach3? If so, how are you ramping into stock and what settings are you using? Can I have your post-processor settings? If this is a know Mach issue, does anybody know a work-around or what might cause lost steps while helixing or pocketing or circling or am I looking at the computer funny and it hates me for it? Have others fixed this issue by installing a dedicated parallel port card in the PC? I've also ensured the parallel cable is away from electrical interference.

FWIW, the Tormach controller is on a UPS, no USB hubs or keys (cheap usb keyboard and mouse, wired, plugged into the front panel of the PC). I've uninstalled and reloaded Mach, acts the same. Booyah.

2.5mm is a pretty big error. I use HSM, Tormach and mach3 often. I am using a good full version of mach3 and not the Tormach version but I SERIOUSLY doubt that has anything to do with it.

Send me your email and I will email you my post file since I don't know how to upload to here

One thing to try is to increase the allowable deviation from perfect in hsm. I don't have it open so I don't remember the exact terms, but HSM assumes you have a machine capable of High Speed Machining when the Tormach isn't even in the ballpark. My 2014 Haas gets bogged trying to run some of the code HSM outputs, but 15ipm seems like it should be able to handle it unless its a VERY tight radius. I use a large radius and ramp at .05" per step and run at 15ipm minute with 1/4 all the time and don't have any issues on my Tormach.

You can also send me the gcode and I can run it on my tormach and Haas in the morning and confirm if it is a control issue or not

[email protected]

Ok, so a test. When I zero the machine, put a dial indicator on the table at zero, run this code, Z wanders down. The first time I ran this, the indicator says zero is 0.008" too low. Run code a second time, without re-zeroing, indicator says 0.028" too low. OMG.

%
O28- OUTPUT CENTER KEY
(T1 D=12. CR=0. - ZMIN=-0.5 - flat end mill)
G90 G94 G17
G21
M05
M998
T1 M06
S4200 M03
G54
M08
G00 X48.119 Y-50.6
G43 Z53.1 H01
Z7.1
G01 Z4.6 F750.
X80.358 Z3.474 F450.
G17 G03 Y-49.4 I0. J0.6
G01 X34.644 Z1.878
G03 Y-50.6 I0. J-0.6
G01 X80.358 Z0.281
G03 Y-49.4 I0. J0.6
G01 X57.98 Z-0.5
G03 X57.768 Y-49.488 I0. J-0.3
G01 X57.468 Y-49.788
G03 X57.892 Y-50.212 I0.212 J-0.212
X57.98 Y-50. I-0.212 J0.212
X57.02 I-0.48 J0. F1000.
X63.98 I3.48 J0.
X51.02 I-6.48 J0.
X69.98 I9.48 J0.
X45.02 I-12.48 J0.
X75.98 I15.48 J0.
X39.02 I-18.48 J0.
X81.98 I21.48 J0.
X33.02 I-24.48 J0.
X81.98 I24.48 J0.
X81.95 Y-49.735 Z-0.47 I-1.2 J0. F1250.
X81.869 Y-49.496 Z-0.381 I-1.17 J-0.265
X81.754 Y-49.299 Z-0.238 I-1.089 J-0.504
X81.632 Y-49.155 Z-0.048 I-0.974 J-0.701
X81.525 Y-49.059 Z0.179 I-0.852 J-0.845
X81.453 Y-49.007 Z0.433 I-0.745 J-0.941
X81.428 Y-48.99 Z0.7 I-0.673 J-0.993
G00 Z53.1
M09
M05
M998
T1(LOAD FIRST TOOL)
M30
%



But if I write a simple code and throw the Z axis up and down a couple dozen times, it's still spot on.

This is not the tool pulling out of the spindle, correct?

Nope, been watching for it. The drawbar is tight enough so the power pneumatics can barely overcome the spring washers.

Just ran it on my machine, it's the code. Try outputting in inches instead of metric. Lost 0.0162" first run, and 0.0324" second run.

Thanks philbobb for running that.

I just swapped solidworks/hsmxpress over to imperial in the document settings, output the same code and ran it. I lost 0.016" in Z.

If i run that code at 100% feedrate ((450mm/min zig-zag, 1000mm/min interpolate the circle) Z wanders up 0.060", run the code at 10% feedrate, Z wanders down 0.012". I think the pattern is Z not repeatable after this code.

Seems odd that it is exactly double the second time. What is the pitch of your ball screw?
I was going to ask also if you are using a center cutting end mill and whether you have checked the connections of the ball screw and ball nut to the frame,
motor mount, belts, whatever, to see if there is any lost motion. Is the screw driven by a stepper motor? It may be losing steps due to too heavy of a load.
By the way what kind of feed rates are these? X57.02 I-0.48 J0. F1000.
.

Try the attached post, it's what came with Fusion 360. Rename to .cps.

Is your post outputting a safety line at all? In the beginning it has something like G90 G54 G64 G50 G17 G40 G80 G94 G49

I am curious too why your using a zig-zag ramp in instead of helix?

I use helixes too, but after a helix move, Z height is off. Turns out, after a zig-zag move, Z height is off.

I don't know what version of Mach3 you're running, but I do believe it's at least a couple of years old, isn't it? There were some versions of Mach3 a few years back that would misbehave on certain transitional moves if the velocity and acceleration settings were not the same on all three axes. That bug bit me on the a$$ more than a few times, and was one of several bugs that finally compelled me to abandon Mach3. Are the velocity and acceleration settings for the Z axis the same as for X/Y? IIRC, the bug I'm thinking of would occur when the Z axis velocity and/or acceleration were lower than the X/Y settings, and there was first a 2-axis linear move, followed by a 3-axis arc move, which is exactly what happens at the start of a helical entry move in HSMXpress. I can assure you the problem is NOT in HSMXpress, or the POST.

I would also recommend "air-cutting", and see if the problem still occurs, to make sure it's not just a matter of pushing the axis too hard when cutting. You might also want to try a more current version of Mach3, just to see if the problem goes away. That would be a strong indicator that the problem is most likely in the version of Mach3 you're running.

Regards,
Ray L.

Mach3 version 3.042.029. This is the CD tormach sent me, its a brand new Series 3 mill, a month old.

I've checked the Z axis motor coupling tight and marked the coupling, motor shaft and ball screw with a sharpie, I don't see slippage.

I'm cutting in air now for these tests, Spindle locked out, coolant switch in off.

thanks again philobobb. when i use your post, the DRO Z height jumps all over when it applies the tool offsets. This test code uses tool 1, so 'load' the tool in Mach, zero the DRO and the dial indicator, cycle start, machine moves to tool change ok but looks to be applying the tool offset again when it moves from the tool change down to cut, happens when Mach executes the 'H1' command. Result is spindle wants to cut about tool #1 height above the zero for the test code (should be cutting at -0.5mm Z, not 90 something).

Quote:

---

Originally Posted by ouchmysac

Mach3 version 3.042.029. This is the CD tormach sent me, its a brand new Series 3 mill, a month old.

I've checked the Z axis motor coupling tight and marked the coupling, motor shaft and ball screw with a sharpie, I don't see slippage.

I'm cutting in air now for these tests, Spindle locked out, coolant switch in off.

---

That version is several years old, as the latest version is 3.043.066. I believe 3.042 puts it back around 2011 or 2012. The versions I had trouble with were about that age. Just for testing, you might want to download the current version from the ArtSoft website, install it to another directory, then copy the XML file from your Tormach install to that directory, and see if that will run. With the Tormach installation, there may be more (like screenset files and resources) that need to be copied over, since they do so many customizations.

Regards,
ray L.

Ray, thanks. Duh, I suppose. If I bought some other electronic device that had software I wouldn't use the physical media that came with it either, I'd go download the latest version. wtf me.

Will confirm after pizza.

no no no, don't listen to him he doesn't own a tormach. get the latests software for your machine provided by tormach that you know are recommended by them and warrantied. 3.043.066 is buggy too. download here.
http://www.tormach.com/downloads.html

Personally I would stick with the version Tormach provides.

I have about two years and well over 100 different parts on mine and never a Z issue like this. I use SprutCAM and Vectric Aspire when not writing programs manually.

FIXED

The latest version of Mach3 runs that test code flawlessly. Twice. The motors sound different too, probably updated controls there as well.

It's not hard, mine is now licensed too. If you're interested, just download the new mach3 from their website and install it like SCzEngrgGroup said below in a new directory. In the old PCNCx directory grab the PCNC3-3.xml or whatever file and move it to the corresponding new folder (the file structure is the same, most of the file names are too). This XML file is already setup and tells mach which pins in the parallel port to use and how the e-stops works and all that. The mach3 manual talks about how to do it yourself, but why? There are other config and screen files in the old PCNCx directory, but I think the Tormach skin is kinda jankey and old, but whatevs. If you load in the license CD that came with your machine and browse to the CD in windows explorer, copy the license file into the new root directory that has that xml file and all. That's it.

Seriously, if you guys are using helix moves and things seem strange, try the new mach version. I was losing my mind, the machine said it was where it was supposed to be, the code said go there, the cutter said no. Simple moves too. Oh well, suck. Back to work.

Most of my programs have at least some helical machining. No problems.

Strange stuff.