Loosing steps - don't know why

[phil_o]

I ran a 3D file today and have a piece of kindling to show for a couple hours of work. The piece is not large 8" x 8" x 1" thick. The roughing toolpath ran fine. The finishing toolpath was fine until about 60% through. Then the X axis started to gradually wander to the left. I've cut many 3D files in the same way without a problem. There are no obstructions, the cut was very light, about .03". The travel speed was 200 ipm. I've cut faster without problems. I ran a 1/8" ballnose at 12K.
My machine is a benchtop with a 4G upgrade and I used Aspire to create the cut file.
What could cause loss of steps?

[Brady Watson]

What was your Z axis speed?

Post a screen shot of your VR settings.

-B

[phil_o]

I've attached my VR settings.

Phil

[Brady Watson]

Looks OK - factory defaults.

You might want to change the following:

3D ramp threshold = 150
Minimum Distance to Check = .08
Slow Corner Speed = 45

You didn't answer what Z speed you are running in conjunction with the 200 IPM number for the XY. This is VERY important when doing 3D cutting...

You may find my post HERE interesting in your situation regarding Z speeds.

Just off the cuff, 200 IPM (3.33 IPS) is pretty fast for a relief that is only 8" long. It would be like asking your truck to go 0-100-0 in the convenience store parking lot...While the software 'sorta' ramps down for speeds that too fast for a given distance, it doesn't really do a great job of this on 3D files. You really want to get in the ballpark & especially want to get the relationship between the XY & Z axes correct when it comes to speeds you set.

-B

[phil_o]

Thanks for the response Brady.

With the XY at 3.33 the Z is at .33. Based on the numbers in your Shopbot Web column (2,1 – 2,2 – 3,2 – 3,3 – 5,3) my ratio is not very good. I plan to try 2,2. What do you think?
My Z number came from the tool settings in Aspire's tool database - the Plunge Rate. I didn't realize that this controlled the Z number for the entire cut. I thought it was only for the initial plunge and figured the software handled the rest.
Is there a way to test the settings other than spending two hours cutting the file?

Phil

I just printed and read your article on the Shopbot web site on the VR command, very helpful. I read it before but wasn't sufficiently confident to play around with these settings.

[Brady Watson]

Phil,
I'd try 2,1 to start. If that seems a little slow, then bump it up to 3,2.

Never rely on the settings in any CAM software. It has no idea what material you are cutting, nor if you are running a metal cutting mill or a wood router.

Experience is the best teacher - The more 3D you do, the more you will know what speeds are appropriate.

It's important to realize that every relief is different. You might one day machine a large smooth relief that lacks small details - and that will machine quickly. Then another day you might machine a large relief with a lot of small details which means the tool needs to slow down to pick up all these details - and that machines very differently than a large smooth relief.

-B

[phil_o]

Thanks for the help Brady. Very much appreciated.

Phil

[phil_o]

I just ran the file that I had a problem with and it came out fine - thanks again.

Phil

[Brady Watson]

Great! Thanks for the feedback.

-B