X0 position moves mid-cut

[brucem26]

Software is Vectric Desktop version 10.019
I have created a file to cut out a coaster. It is two sided and is basically a series of open ended vector arcs.
I can simulate the cut in Vectric and all is perfect.
I am using the Mach 2/3 Arcs (inch) *.txt processor which has worked perfectly until now. My CNC is a home built unit.
When I start the cut it created the first 4 arcs as anticipated. When it started to cut the 5th arc the system (on it's own) moved X0 to be almost 2" away from its original X0 position. Hence when it started to cut the 5th arc it ruined the piece.
I opened up the G code. I don't see anything wrong with the G code... Where the 5th arc should have started. I killed the job and hit "Go To 0" in Mach3. To my surprise the display in Mach 3 showed X0 Y0 and Z0 but in actuality the machine went to X 1.850 Y0 Z0
So something mid stream changed the X0 point and buggered up the job. The CNC thought it was starting the 5th arc at X=10.000 but in reality it was starting it at X=11.850 relative to the original X0 point.

Vectric support said "If Mach3 is showing the correct toolpath, the problem is not in the file, but with the machine tool or control software configuration. From your description, your machine tool has lost some steps."
I agree but how is this possible?

Note: When I click to calculate the profile toolpath I get the message:
"The selected vectors contain groups with multiple open contours. These will be cut as multiple open contours and not as a single contour. ...."
I presume that is just the warning that I am cutting open ended vectors which is what I want to.

Any ideas? I am really at a loss here. Many thanks.

[sharkcutup]

What is your cnc machines X-axis cutting length. What is the size of your project along the X-axis? I am thinking lost steps too!!!

Are you sure it has ruined the piece --- Reason for asking: Sometimes the CNC machine g-code has things in a skip around order it is not always 1, 2 ,3, 4, 5 it may be 1, 2, 3, 4, 9, and later in the g-code come back to 5. What did you see in the Vectric preview? This is always representative to what the g-code. Does it skip around or does it actually cut in the order in which you are thinking - straight forward one after the other?

On the other hand if the home position is not zero it has lost steps somehow? Please answer above questions.

Sharkcutup

[TReischl]

So. You looked at the g code and it is fine. You looked at the preview in the software and it is fine.

What makes YOU think that the machine is not losing steps? Just because?

[ezurick]

I've had similar results of losing the XYZ due to static... once I grounded my machine bed, spindle, and controller I rarely have any issues. One thing that could cause the Z to lose it's settings is the clearance when it starts. If the spindle is clipping the top of the clearance, it will also lose its zero...

[Adrian]

Any reason for cutting it as a series of open arcs rather than closed?

[martin54]

From your description the machine lost steps, there is no feedback on a stepper motor so the machine isn't always where the control software (mach3) thinks it is, this is why when you sent the machine to zero the axis was not where it should have been.
There are lots of reasons for lost steps & it can be trial & error to determine where they are being lost, things to look for are axis binding, slipping couplings, to aggressive cutting (to deep or to fast) acceleration/deacelleration settings & static as has been mentioned to name a few that spring to mind.
Have you checked that it cut the first 4 arcs perfectly ? It may be that it hasn't & the loss of steps has been gradual but not noticable at first glance on the first 4 arcs. If it has then I might be looking at binding or the acceleration settings in mach3 first.

[Leo]

With limited information about the machine or cutting parameters I will agree with lost steps.

[brucem26]

Thanks to all.
The machine has a 24 x 48 bed. This project is only 12" long x 5" wide.
The piece is definitely ruined... after it finished the 4th arc I could see it "jump" an inch and a half or so and start to cut the 5th arc (correct Y position but X messed up).
The strange thing is that I can carve any other shape and design and it does it flawlessly. It is ONLY when cutting these open ended (non-closed) vectors that it goes awry. I have never cut open ended vectors before.

Static is ruled out. Most of the machine is plywood and I have the spindle, the gantry, the bed and the electronics enclosure all grounded together.

I even tried creating 8 separate toolpaths in Vectric (one for each arc) and then combining them when saved as GCode. This time it cut arcs 1 through 7 perfectly then "jumped" just before starting to cut the final arc #8
Conclusion it is definitely random when it happens and the amount it "skips" is random too (up to almost 2")

I really don't think it is skipping steps...
* Why just on non-closed vectors
* Why always the X axis
* Why not gradual skipping... it's all of a sudden.

Side note: Isn't there some way to attach an image on my computer to these posts? When I click "Img" above it only accepts a URL.

[Adrian]

You use the upload attachment button underneath where you type your post to upload a picture.

If the g-code is correct and the preview is correct then it's the control software setup or the machine itself. If the g-code is correct then the Vectric side of things is out of the picture at that stage.

I know it doesn't answer the question of why it's going wrong but why are you cutting them as open ended arcs rather than closed arcs?

[brucem26]

These cannot be cut as closed vectors (at least I don't see how).
Each of the 8 arcs has a profile toolpath to cut on the outside. If they were closed I wouldn't be able to have the bit cut on the "outside" each time... see below.

[Leo]

after it finished the 4th arc I could see it "jump" an inch and a half or so and start to cut the 5th arc (correct Y position but X messed up). This time it cut arcs 1 through 7 perfectly then "jumped" just before starting to cut the final arc #8
Conclusion it is definitely random when it happens and the amount it "skips" is random too (up to almost 2")

I really don't think it is skipping steps...
* Why always the X axis
* Why not gradual skipping... it's all of a sudden.

Boy, this sure sounds like missed steps to me. Your description here is a really good description as to how it happens, and yes "random" is common with missed steps, so is one axis direction, as is suddenly. All of that sounds like missed steps.

Did it also make a grinding sound like gears that were not meshed well, or severe chatter?

Did your "Z" axis hit the top of it's stroke?
Is there an obstruction on the ball screw, guide ways?
What feed rate are you running?
What size stepper motors do you have?

Is is very unlikely that the problem is in V-Carve. Not being defensive here, but usually the answer is elsewhere.

[scottp55]

Just curious,
What happens when you do an air cut....AND Profile cut ON the line?

A preview in 3D view with toolpaths checked would be of help possibly as well.
scott

[martin54]

I am with Leo, still sounds more like missed steps than anything else.

If the toolpath preview in the vectric software is good & your g-code looks to be good then it is more likely to be a machine issue or something in the mach3 set up

How have you grounded the parts that you have mentioned? Are you sure you haven't created any ground loops that would cause electrical interference ? Do you have any other machinery that starts & stops that may cause interference ?
Do you have a dust extraction system on the machine & have you earthed wire that? I am not saying that it is static causing the problem but don't be to quick to rule it out unless you have checked absolutely everything

https://www.shopbottools.com/ShopBotDoc ... 8%2007.pdf

[brucem26]

Success!
I changed the toolpath to a profile cut ON the vector instead of outside.
I then changed the series of open vector arcs by closing them up to become a closed vector.

Making no other changes I ran the cut again and it performed exactly as expected! The machine retained it's X, Y and Z position.

I am in no way inferring that Vectric is handling the open vector cuts incorrectly (because they always appeared correct in the 3D preview) but why did just changing it to a closed vector fix everything?

The motors have lots of power (1200oz X axis and 480oz Y and Z axis). Nothing is grinding and there have not been any other cases of missed step with anything but these open arcs.

I will keep investigating. Thanks to all for your valued input, I really appreciate it.
I wonder if my choice of GCode post-processor might have an impact. I am using the standard Mach 2/3 Arcs.txt one

[TReischl]

If you get back to investigating this with your original file that jumped there is a very easy way to figure out if it lost steps or not:

Mark your XY zero on the workpiece. Run the job. When it is finished issue the command G0X0Y0 in the MDI text block in Mach. The machine should go to the zero you marked. If it does not, you have lost steps. Simple as that.

Mach3 actually runs based on machine coordinates, not program coordinates. That is why it is important to home the machine when initially powered up. IIRC Mach3 normally uses G54, this causes the math to be done internally to get to the correct machine locations. All of this is so that various work coordinate systems can be used and to make it easy to pick a zero on the part or a fixture location.

Changing a program as you did and then asking why it did not do it in the new program is not good troubleshooting technique. Not being snarky. The way to figure out what is going on is to NOT change the program if you know the code is good as you have stated. If you can, posting the bad program g code would help. A lot of us read it like a cheap comic book. The other thing doing that would do is allow some of us to load it up and see how it runs on our machines.