V-Carve Pro Air Cut

[robbwk]

Environment: CNC Router/mill - 2.2Kw Spindle - Hardwoods only - MASSO G3 controller (Config file version 3.42.2) and V-Carve Pro 10.18.0. I have the correct post processor installed - (FYI only: I use Imperial measurement).

I have a weird occurence taking place. At a point in the job the Z-Axis changes from a negative to a positive position. For instance, I have a test file: testing.crv (which is just the word' Testing') which uses a Carbide V60 degree, 3F Trend .57" dia' bit and is in the Toolbase using appropriate vendor settings. The depth of cut for this file, at maximum, is 0.125". The size of the material is 6" X 4" X .75" and is Oak. I first Home the machine correctly, I have then set the job 'Home', bottom left and at the material surface with all axis at 0. I start the job and all goes swimmingly until the bit completes part of the text 'TEST'. It should go to the 'i' and it does but, the Z axis has now risen from the correct depth (in the Gcode for the previous 't') to a positive position and, consequently, it air cuts the rest of the letters 'ing'.

I have a correctly set up machine. The spoilboard has been surfaced and checked for level by measuring the distance between the spoilboard surface (all four corners and center) and the bottom of the spindle at a set height. The X axis gantry is level across the entire table. The whole system is only a month old and has, virtually, no usage other than setup and testing. I have configured the controller using the latest software update direct from MASSO. The Z-axis is correctly setup and has been checked using MDI to ascertain that a command results in a correct postioning of the Z axis. Homing work correctly and V-Carve 'appears' to be creating accurate measurements and Gcode using the MASSO/Vectric post processor.

Here's a thing: As the Z axis moves into a positive position during the test job I hit the E-Stop. The Z axis on the MASSO is showing a correct position as -0.0825" at the time I stopped the job but, the position of the bit is, clearly, above the surface of the material at about the same value but a positive value of 0.0825" (approximate, as it is difficult to measure accurately).

I have been working with my CNC vendor to try and resolve this anomoly. Mechanically, all is in order. I thought that this Forum might be a good place to ask for help as this may be a V-Carve 'problem'. Either one I am creating or V-Carve has a bug(?). I am also posting a similar message at the MASSO website forum.

[SRiddle68]

A simple check you could do to point to the Vcarve software or the CNC controller software setup is to scroll through the G-code and see what Z depth is being called out for around the point you have the jump in position. If the Z depths all look good then I would say it is something to do with the controller software and the CNC, not the Vcarve G-code. One other question I would have is this a repeatable issue? Can you reproduce it 3 times in a row with the exact same result? Machines "usually" are very repeatable if they are working properly. They will do the wrong thing again and again. One other possibility, that I have experienced, that is similar, is a loose cutter. It was fairly tight but when it did a deep plunge it was enough to drive the tool up in the collet a little and then all my cuts were shallow from then on. I was using a 6mm shank cutter in a .250" collet. It would tighten down but I had to go about another half-turn or so on the collet to tighten down. I think it may be tight but it is more of a line contact and not a surface to surface contacts like the 1/4 collect and 1/4 shank tool would be.
Just my 2 cents. I hope it helps and wish you the best of luck with this. They can be a bugger to figure out some times.

[robbwk]

Hi and thanks for your response. Very grateful for any help offered. Your 5 cents is worth a hundred bucks to me.

I have checked the Gcode at the point (and beyond) where the spindle rises. It is what it should be -0.0825". The problem is repetative using different V-Carve files. I have also taken the trouble to move the work-piece to different locations on the spoil-board for obvious reasons. I did check the cutter/chuck tightness - it's fine. I have taken a video of the problem in action. If you want to view to, maybe, switch on a bulb in your head, let me know and I will send you a link to my business web site where there is a private link to the video. It's not a brilliant piece of filming as I don't have a Camcorder. However, it does show the damn thing rising from the job. Thanks again.

[mtylerfl]

Hi,

I don’t see a link to view your video. A picture is worth a thousand words - but also seeing your actual Vectric project “Testing” file (NOT your GCode!!) might be worth two thousand.

Please upload your file and post your video link. (If your file is over 2mb in size, you’ll need to use a free service such as DropBox to upload your file to, then copy/paste the download link here.)

Thanks!

[robbwk]

I attach the job file.

The link is http://www.wessexmillwork.com and scroll to the bottom of the page (continuous page) and click on the Wessex Millwork logo in the footer.

Today I swapped the Z axis stepper motor for one of the Y axis stepper motors. When I ran the Tester job the result was, sadly, the same as in the video.

Grateful for your help.

Thank you.

[Adrian]

Looks to me as though the dot on the i (56 second mark) is too much for the z axis at the plunge/feed rate/pass depth (you can hear it struggling) and it's losing steps so the physical position of the bit is higher than the controller thinks it is.

I'd step the pass depth down so it takes multiple cuts on the dot rather than trying to plunge it all in one go.

[SRiddle68]

I agree with Adrian, it looks like your Z axis lost some steps in that plunge cut. You must have regular steppers without any position feedback to detect lost steps. That is how my CNC is and I have had certain parts lose position in the Y axis. For my new "homemade" CNC lathe I purchased the Chinese steppers with drivers that have encoder feedback built into them. They throw an alarm if they do not get to the commanded position. They are also a ton faster than a normal stepper. They are basically like a servo.
Hopefully, a few tweaks to your feeds and speeds and you can get past this problem. I just upgraded from Mach 3 to Mach 4, on my router, and had to retune all my steppers and I found that I had to reduce my acceleration on my Z axis because it was causing some erratic behaviors. I just slowed it a little and my problem went away.
Scott

[robbwk]

I want to thank everyone on this forum that have taken the time and trouble to think about my difficulty and offer solutions and advice. I am very grateful to you all.

The solution was provided by a person on the Masso forum who owns a similar machine. It is in line with the advice from you folks. He gave me numbers which I applied and the result was that the system is now working as perfectly as it ever has. Probably needs a bit of tuning over time but, I'm very pleased with what it is now able to do. This is not my hobby, it is my living and this machine must pay for itself and make me money or it goes to the tip. I built this system from a kit and I had been blaming myself for the problem. The actual problem was that the vendor had sent me a config file for the machine which was created in metric and, although I live in the UK I use Imperial measurement. The translation was not accurate. I don't know why the vendor delivers only metric settings but, I suppose because I'm in the UK the assumption was I would use metric. I don't. I design in Imperial and work in Imperial. I do refer to metric now and again but, I'm more comfortable using Imperial measurement. The accurate setting for my Heavy Mill is:

Pulses / revol = 2000
Max feedrate = 15in/sec
Acceleration = 1in/sec^2
Travel Min = -4 in
Travel Max = 0

Thanks so much for your input. I hope to reciprocate by contributing to this forum as time goes by. Have a nice weekend folks.

[Adrian]

Glad you got it sorted in the end. As you get more into CNC you'll develop an eye and ear for when something is not quite right. I flinched as soon as I heard the machine trying to cut that dot.