Trouble with TCPC

After two days of struggling to get my machine to run a program with TCPC, I finally got an almost good part. Frankly it’s close enough that the minor issues I’m seeing with it could be down to having my WCS not perfectly set (manual touch off with a paper shim). So I was all set to declare victory when I decided to push my luck. I drew up a very simple part. Just a cylinder pointing along Y with a flat on the front and back surface and a through hole. The part is held in the standard vise which is oriented with the moving jaw pointing away from me so the material is centered on the table in Z but offset from center in X. Zero is set on the top, right, front “corner” of the round bar. The first operation to flatten the front face runs fine, the table spins 180 in B and the second op, which should do the same thing to the backside of the part, is nowhere near the part. The Z height is so far off the tool never touches the part even at the deepest cut level. Didn’t bother to continue with the program to see what would happen with the through hole since obviously something is wrong.
I’m at a loss to understand what is happening. I assume I’ve done something wrong in the CAM but truthfully, don’t have the slightest idea what that could be. Any suggestions or guidance would be greatly appreciated.
In case anyone is wondering why I didn’t just mount the material in a collet, because of my struggles over the last couple days with TCPC, I am deliberately creating a scenario that requires it so that I can (hopefully) understand it better for when my parts are less simple or my material is less round.
Picture attached is the test part showing my WCS point in case my description was unclear.

When you set your Z axis work offset did you make sure the proper tool was active before performing the touch-off and setting the DRO? It sounds like your TLO offset has not been accounted for (or the wrong one was accounted for).

Also, you can still mount your stock in the center of the table using the ER40 collet fixture and use TCPC. As a matter of fact, unless your WCS origin is set at the center of rotation (we call it the B-table offset), you have to use RWO or TCPC. So if you mount round stock with the ER40 collet fixture and place your WCS origin on the top of the stock in your CAM, then you only have to set the Y axis work offset. This will still require TCPC to work properly, but it reduces chances of human error since you only have to set one work offset. This method would void the potential TLO problem mentioned above since you would not be setting a Z work offset.

Thanks for the suggestions. I am fairly confident I had loaded the tool and set its offset immediately prior to touching off Z but the behavior certainly would point to that being an issue. I will try again and see if that fixes it. Wouldn’t be the first time I’ve made that rookie mistake but it’s certainly been a while.
I wanted to run a worst case scenario setup to really check that the TCPC was working as expected. The only material I have that isn’t metal is round delrin so even though I could have put it in the collet I opted to go with the vise to get some real offset after rotation.

I had a really long response written out before I suddenly had a thought which proved to be the cause of the problem. For no particular reason, I oriented the vise 90 degrees off from where I wanted it. Rather than changing it’s position, I simply rotated the B axis 90 and set that position as G54 B0. It’s this offset that seems to be causing the problem, though I don’t really understand why. For the record, I did double check my Z offset and tool length but that was spot on.

I’ve attached the program in the hopes that someone can figure out what’s going on. Use the following offsets taken directly from my machine setup:
Tool Z offset: -3.3981
X 0.407
Y 1.6215
Z 0.5031
B 90
Skip ahead to line 4874 for the action. You’ll see the toolpath, which is positioned slightly forward of center in Z and off to the far side of center in X. When the table rotates, you’ll note the new toolpath is roughly centered in X but quite a bit farther forward in Z.

Now run the simulation again but this time remove the B offset (set to 0). This time you’ll see the initial toolpath in the same place BUT after the table rotates, it’s on the other side in X at the same Z position which is where is should be.

So now my question is, is this a bug in the machine control software or is there something else going on here? I, of course, realize the simple work around to this is just to re-orient my vise and remove the B offset but I am curious what this means if there is ever a true need to offset B, to tram in a part for a second op for instance.
1001.ngc (185.8 KB)

Unfortunately, we don’t currently support work offsets with A or B values other than 0 when using RWO or TCPC. This is likely why the post processor isn’t adding the RWO codes around your tool paths that are at A0 B0, which would be necessary to perform the transformation. This is something we would like to improve at some point.

Well I have an answer at least and I know what not to do going forward. Thank you for the info.

A probe should be included with this cool machine - imho!
Ok, it costs about $300 but makes the work a lot faster and causes fewer errors.

PS: knowing absolutely nothing about NGC files, it took me several days to get it working for all A/B position combinations…

I certainly don’t disagree with the value of a probe. However, in this case it wouldn’t have been helpful. After several days of troubleshooting and working with the crew at Penta I finally have a solution. Turns out my X and Y calibration was off. X by about .014” and y by another .004 or so. No idea when or why the calibration was changed as I’m the second (maybe third?) owner of the machine but getting it dialed back in has solved the problem. I now have less than .001” of positional error in both axis which is good enough for what I believe the machine to be capable of.

ok. Is there an official procedure, to find out such inaccuracies?
We should probably be able to periodically check these values…

quote=“WilWeber, post:7, topic:588, full:true”]
…but makes the work a lot faster and causes fewer errors.

But only if you always also look on the back of your model, if you x-probe from the back.
I forgot that there was a raised area in the back and just destroyed a tool.
John, please add a camera or a mirror :wink:

There is but it’s fairly lengthy and requires a specific test program. I’m not really comfortable trying to post it all given the potential to create problems for people.
The easiest way to check if you have a problem would be to bore a hole halfway through a piece of stock, then rotate it 180 in B and bore the same hole halfway through again. If your X calibration is correct, the two holes should line up more or less perfectly. In my case there’s was about a .030” offset between the two sides.

1 Like