Pitting & dimpling - need advice

[MDCochrane]

I'm getting surface pitting on the HDU I'm carving. (See attached photo, which shows about a 3"x4" patch.) I then have to sand it out by hand, which on a 3'x4' surface takes me nearly 3 hours. I've been a ShopBotter for less than a year and need some advice from you guys who have been at this for years.

I'm carving a 3D wave pattern into 1.5" thick, 15lb. CoraFoam (green Duna Board). The depth of the cut varies continuously between 1mm to 15mm. Here's the data you're sure to ask me for:

CNC: PRT96 with v4g update.
Comm rate: about 70% efficiency
Feedrate: 85 mm/sec
Plunge rate: 15 mm/sec
Router: Porter Cable 3.25 hp, selectable speed
RPMs: 19,000
Bit: 3/8" ball nose, flat, two flutes (Whiteside 1407)
Stepover: 10%

I'm guessing that my problem is a mismatch between the feedrate and the plunge rate. The Duna technical rep. recommends a faster feedrate than I can run with a complex 3D carve like this. My electronics in the controller on this table are pretty old and I get increasingly dropped lines of resolution with every step I go up past 85mm/sec. The Duna techs don't say anything about plunge rate, however, and that's where my question lies.

How fast can I set the plunge rate before something pops? Is there a proper ratio between feedrate and plunge rate that better ensures smooth transitions?

Here's what I THINK is happening. The cut is an X raster motion. The pitting is happening on the climb and decent of the wave walls. When cutting a few inches along a wave trough, the machine's velocity speeds up and there is little, if any, pitting. When it comes to a steep climb or decent on the Z axis, the x velocity slows down, gets a bit jerky, and that's where the pitting happens. I'm thinking the plunge rate is slowing down the feedrate in those areas and the pitting is the result of the bit tip spinning too long in each step as the machine makes the climb or decent.

Can I match the plunge rate to the feedrate at say, 65mm/sec so that the x axis velocity is a consistent speed through the steep parts of the cut? The HDU cuts quite easily, but is a very high plunge rate a crazy thing to do to my equipment? The whole job is a side cut. There isn't anywhere where the bit drills straight down.

Thanks for your wisdom, those of you who have been down this road -- new to me.

Mike

[Brady Watson]

Go read this: http://www.shopbotblog.com/index.php/2008/03/a-ramping-the-vr-command-and-how-to-tune-your-tool-for-maximum-performance/

Then adjust your SCS accordingly. I would try machining at MS,75,50 and see if you get an improvement. I would also set 3D Threshold to 150. If it machines OK @ 75,50, try 125,75 - although this may be too aggressive for this relief - use YOUR best judgement & err on the side of being conservative with your speeds. That should cover the software side of things.

I would have the control box on & grab the Z axis and wiggle it up and down, move it up and down with the keypad and wiggle it around (pretend you are a gyroscope pulling it in all directions) - listen and FEEL for any slop. At first glance it appears that you have a little backlash in the Z, but this could be a reverberation of the Z axis since the XY:Z ratio is a bit too lop-sided with the Z speed too low.

Gauge what the Z can do - then match XY speed to a proportion I've found to work, listed in the article linked above.

-B

[ron_moorehead]

I have never cut HDU, but I have cut some pink foam. and have done a lot of 3D cutting. I have never seem this, looks like it's cutting small holes for the profile. I have a couple of question how are you holding down the HDU? Have you check for any loose pinion gears and is the Z axis binding in any way. I would turn the power off to the motors and move the Z and X and Y around and make sure it's moving freely and not binding. Last thing how was the 3D file created for you.

[MDCochrane]

Spot on, Brady! Your article is exactly what I was looking for. I'll tune the VR for 3D cutting and set the Z rate to something reasonable like the 75,50 mm/sec you suggested and let you know what happens. I'll back on the machine tomorrow.

[MDCochrane]

Good idea, Ron, to check for slop in the pinion gears, as well as for any binding. I'll do that. I think the more probable culprit is that my move speeds are so out of balance, as Brady mentioned. I haven't had this pitting on other 3D objects I've cut in wood. I think the speed ramping caused by my low Z speed is heating the HDU in those places where the X speed is pausing to allow the Z to catch up.

I made the toolpath processor file in Cut3D by Vectrics. I made the 3D surface myself in a modeling application named TouchCAD.

[MDCochrane]

Just checking back with you, Brady.

I made the VR adjustments you recommended in the paper. I then bumped the feedrate up to 75,50 on a test piece and it looked much better -- almost no pits or dimples. I pushed it up to 125,75 and I couldn't see any loss in quality, so I ran the job at that rate. If I would have had more time before the deadline I would have tested higher rates with the Z, but I didn't want to get outside the ratios you mentioned in the paper. I'll do more testing later.

There is so much climb and descent going on that I don't think the XY feedrate ever reaches 125mm/sec (5"/sec) on the job. The speed ramping is still obvious but the smoothness of the machine was greatly improved. Very little vibration by comparison to when the Z rate was so low. The 48"x84" cut took about 13 hours. I still had to hand sand but it was much easier without the pits.

Attached image is the sign substrate, cut and sanded.

Thanks!

Mike

[chiloquinruss]

Just think how long that would have taken with a hand router! Oh wait, you can't! :D Looks great, nice pattern. Russ

[myxpykalix]

You may also want to adjust your safe Z height to just above material surface when making your file to keep the rise and descent to just a bit above material to speed things up.

[Brady Watson]

Mike,
Thanks for reporting back. If you find that the tool never gets up to full speed in XY because it is waiting for the Z, pull back the XY speed to match the Z. The key to speedy 3D files like this is not to trigger ramping.

-B