Finish Quality

Michael J Starry · Post by **Michael J Starry** » Wed, Nov 22 2006, 2:35PM

What kinds of finish do you all achieve when using your 5 axis machines?
We cut plastics here, ABS, Poly, HMPE/HDPE, Etc. and we seem to have a lot of difficulty achieving a decent cut/finish. Tend to be a whole lot of chatter and tooling marks. Not only on curves, and radii either, though mainly.
As a standard, we cut at 18000 RPM and the max I have been able to cut is 200 IPM on a totally flat, straight cut. Typically we end up near 125 IPM or slower to get anything near an acceptable finish. Using double O Flute Straight Flute.

Ryan Hochgesang · Post by **Ryan Hochgesang** » Mon, Nov 27 2006, 4:51PM

Mike,

If cutting on a five axis machine it is always best to fixture the material being cut, as high off of the table as possible, keeping the z axis as close to it's mid travel as possible. If the z axis is fully lowered with the router being farthest from the mounting area on the z axis tooling plate, there is a lot of leverage that could cause some tool tip movement resulting in chatter. Also, it is very important that the material be secured as snug as possible. If there is any part movement, you will get chatter. Cut quality is also affected greatly by type of toolpath used when programming. It is best to use arcs and straight lines when specifying tool paths. It is also important to use the tangency factor (G09F8 usally best, Range from 1-15) and Acceleration factors (G802 usally best, Range from 1-9) when dealing with certain types of cut geometry that may have directional changes. Typically the double \"o\" flute style tool works good for plastics. I've trimmed parts at 300-400 IPM and acheive smooth edge finish on the parts. On certain materials I've used a 3 flute, low up-spiral type tool to get good cut quality. You may what to give that a shot as well.

I hope this information has been helpful. Please feel free to contact programming support at Thermwood for any addition questions you may have.

Michael J Starry · Post by **Michael J Starry** » Fri, Dec 08 2006, 11:02AM

That is why I am worried about it. We fixture very high to compensate for the potential chatter issues, i have tried evey combination of G09 F# that I can come up with as well as the G80# with little to no improvement.
Our fixturing is usually pretty tight, so our parts have little to no room for movement.
I am left with some shots in the dark as far as cutting tools go, so I will be experimenting with those next week.
If that fails, I think I will have to relegate myself to the fact that our machines are worn to the point of no return, and live with the chatter issues.
I convert everything from splines to arcs and lines in Mastercam before I program parts, as I know about the limitations of splines. So I have ruled out that factor as well.

Matt Quarles · Post by **Matt Quarles** » Fri, Dec 08 2006, 4:00PM

First thing I would try is replacing the axis belts. Then use an indicator and check for backlash in axis 4 and 5 if this error is large you are looking at an axis rebuild possibly(worm gear, bronze gear etc,,..). Next thing is checking for lash in the x,y,z. I just went through this with a machine and we ended up replacing gears, screws and bearings. Good luck

Ryan Hochgesang · Post by **Ryan Hochgesang** » Mon, Dec 11 2006, 3:11PM

You can try using these AFL statements within the CNC program to further adjust Gains and Accelerations if your unable to acheive the cut quality your wanting:
Note: the following info. are samples only, info in parenthisis is explanation of that in brackets.

[WRITEGAIN (6,.3)] (Ranges 0 to 1.5, Recommend no lower than .3)
[WRITEMAXACCEL (2,10)] (Ranges 0 to 15, Recommend at least 10)

Michael J Starry · Post by **Michael J Starry** » Wed, Dec 27 2006, 11:23AM

We checked for backlash, and are at about .003, so that isn't the cause. Belts are good. I really believe that it is just a matter of tooling and lack of maintenance at ths point. I will be trying new tooling this week and will update then.
Thanks for all the help and suggestions guys!

Merry Christmas

Michael J Starry · Post by **Michael J Starry** » Tue, Jan 30 2007, 1:36PM

Just an update.
I have tried all kinds of different tools now to no avail.
Different brands, styles, more flute, less flutes, o flutes, upcut, downcut, compression, all with roughly the same results.
I guess we will just continue to deburr and sand the crap out of everything to compensate.

Ryan Hochgesang · Post by **Ryan Hochgesang** » Wed, Jan 31 2007, 4:04PM

If you will send a copy of your Mastercam drawing along with the cnc code your running to: program@thermwood.com , I will be glad to take a look.