V90 stalling/cutting error

[dustincowell]

Hi,

I'm having a problem with cutting on my new Probotix Fireball V90 and I have no idea what may be causing it. Part way through the cutting, the CNC stalls and changes cutting locations. Please excuse me for not knowing all the right terminology to describe the problem as I am new to CNC in general and just finished setting up my V90. I consider myself advanced with computers and intermediate with woodworking, just new to CNC. I took a video of the problem figuring that it would be a lot easier to show what it's doing than to try to explain it. Here's a link to the video on YouTube...

Please let me know if anyone knows what could be causing this problem.

Thank you very much in advance!!!

Dustin

Similar Threads:

• CO2 40W LASER ENGRAVING CUTTING MACHINE ERROR ID:1
• Need Help!- cutting Data won tranfer via USB cable to laser engraving machine comes up with error
• Problem- Yaskawa servo with Syntec controller 0.4 mm error cutting
• DNC stalling
• Error cutting on a z level pass

[dustincowell]

I slowed down the x and y to 30 ipm and slowed down the z to 15 ipm last night. I'm happy to say that fixed the slipping!!!

I have two other issues now though and wondering if you know what I can do...

1. I cut .75 inch thick poplar at .1 inch passes. It made 8 passes to cut all the way through. The end result pieces have small lines running along the side from each pass. Is it possible to clean these up with the cnc or have it cut in a way that I will get nice smooth sides... or at least sides without lines?

2. The end result piece ended up being a lot smaller and thinner on the outside profile cut than on the vcarve design. In vcarve pro it was the right size when I traced the imported bitmap with the vector tracing tool. I did also set the tool diameter to .125 before generating the tool path. Any ideas what would be causing this or how to fix it?

Thanks again!!!

[ger21]

1) Check and make sure that your spindle is perpendicular to the table in both the X and Y directions. If it still gives you the lines, it may be the tool or spindle flexing.
In V-Carve pro, when you do your 8 passes, offset them a small amount, maybe .005-.01. Then do a single full depth pass with no offset to clean up the lines.

2) You may need to adjust your steps/unit if the machine is cutting undersize. You'll probably want to do some test cutting and see if everything is consistently undersized.

[br1]

One axis or all could be flexing, or the tool may be flexing as well, leave .01 or so for a clean up pass at full depth, it could also be a small amount of backlash.

[louieatienza]

1. If your Z is not trammed properly, meaning perfectly perpendicular along both the X and Y axes, then, you may get these lines on the sides. You can get a piece of 1/4" drill rod, chuck it into the router, and use a small precision square to check. Having said that, you can tell VCarve to leave .015" or so on y oru profile cut, and then run one finish pass at full depth to clean up the edges. I would use the lead-in and lead-out to minmize any witness lines.

2. You should specify inside cut for the inner profile, and outside cut for the outer profile.

Really I would use a 1/4" tool to cut something this thick. If I wanted the sharper inside corder that the 1/8" bit would provide then I'd use a 1/4" bit to cut the window leaving .010" or so, and follow up with a 1/8" bit to clean up the corners.

You don't mention the feedrate on your video. Of course slowing things down can help, but I would check your acceleration. You may need to lower it; with your PSU and steppers you should be able to cut at a faster clip (leadscrew depending...)

Another thing - don't use MDF for a teething ring; the gue normally used contains formaldehyde, and if this is Chinese MDF sold at Home Cheap-O God knows what other chemicals are in there. Oak, walnut and cherry contain tannins that some can be allergic to.

Finally, don't run your router full-tilt. Making dust causes the bit to heat up excessively, which causes premature wear. I think your breakage was a result of lost position, causing your bit to plunge too deep and take too deep a cut for its diameter. It will take a couple broken bits and a lot of test cuts to get the right feeds and speeds, but you want to run as high a feedrate as possible with as low a router RPM as possible. Also, you should leave tabs, or onion skin, or other method to fix the slug and part from moving when cut through. The part can shift and jam the bit causing it to break or at teh very least leave a gouge.