Tooling marks, help...

[tim_mcknight]

Let me preface my post by admitting I am a TOTAL noobie with my "Buddy". It has been a long day in the shop today, 16 hours later, I finally cut three guitar finger boards (2 ebony and 1 Rosewood). The top surface has a 16" radius convex surface. I just can't seem to get the tool marks out of the radiused surface. I tried all sorts of cutters.

Flat bottom 1/2" diameter 4 flute end mills left the worst ridges. I ended up using a 3/4" diameter CMT bowl and box router bit. I tried 1/2" to 1-1/2" ball nose router bits and they had a lot of tear out. The bowl bit had the cleanest cut but still left pronounced step over ridges. I varied the step over from 3% to 8% but it did not make a discernable difference in the surface texture. I cut it in the X (long) direction (along the grain) on my Buddy. I tried 2 - 5 IPS cutting speeds and used a constant 12,000 PC router spindle speed.

Any suggestions would be greatly appreciated.

[richards]

Tim,

How far apart are the "ridges"? At 12,000 RPM and 5-ips (300 inches per minute), the marks would be 0.025 inches apart. I often get tooling marks on my router table when I round-over an edge and move the material too quickly past the cutter; however, the ridges that I get with my PRT-Alpha are not tooling marks. I constantly get ridges about 1/8-inch apart. With the 7.2:1 geared steppers, the depth of those ridges is very shallow and they are easily sanded off (100-grit cleans up MDF in one or two strokes), but they seem to be inherent in the design of the machine. Some of the marks seem to be mirror images of the ripples in the V-rails, other of the marks just seem to appear for no reason.

They were a frustration for months while I tried various cutters, various speeds and various angles, but nothing eliminated the ridges completely. Now I just know that I'm going to have to lighly sand most parts.

A few days ago, I finished a 2nd batch of Doll Cradles for charity that took six sheets of 3/4-inch MDF and eight sheets of 1/2-inch MDF. When the parts were stacked, the ridges matched almost perfectly on the 192 end pieces, 192 side pieces and 96 bottom pieces. Since those parts were cut from full sheets, the surface irregularities on the rails couldn't have been the cause.

[tim_mcknight]

There are no tooling marks per se in the direction of the cut. The ridges appear to be from the step over. There are a LOT of parallel lines on the surface left from the .060" step over.

[beacon14]

3% to 8% of .75" equals a .022" - .06" stepover. The bowl bit has a flat bottom and radiused corners, right? And the workpiece is a gentle (16" radius) convex surface. If you think about how a flat bottom tool interacts with a convex surface you realize that only the very corner of the tool can ever touch the surface (except at the very highest spot). So you are essentially using the radius of the bowl cutting bit, if it's a 1/8" radius that's the equivalent of a 1/4" ballnose bit, so your .022" stepover is closer to 10% than 3%.

Try stepovers in the range of .006" - .008" and see if that makes a difference (other than in machining time of course). Also try new, sharp, high quality ballnose bits instead of the flat bottomed bowl bit.

[tim_mcknight]

I am using a brand new CMT bowl bit and it "looks" like it is round with no flat spots on it like a typical bowl bit. There is a 1/8" gap in the center between the two carbide cutting surfaces though so this may be the flat area you are referring to? I will need to make a test cut on a flat surface to verify the cutting profile.

What diameter ball nose bit would you suggest David? Would a solid carbide end mill or a router bit work best? Do you have any bit sources that you would suggest?

[beacon14]

Normally on 3D work a smaller diameter bit will yield better detail, but in this case a larger bit should give smaller ridges and a smoother surface. I'd go with a 1/2" or even a 1" bit if I had one on hand.

Do a search of this forum for router bit suppliers - there have been several threads on the subject.

[Gary Campbell]

Tim...
In some cases the software doesnt do the best job when it is asked to use a bit that is out of the norm. We as operators sometimes forget to take the time to exactly put in the correct parameters both for the bit and for the toolpath. With the type of large radius'd surface you are trying to create, anything but the best combination of these parameters will result in exaggerated toolpath marks.

I agree with David on the bit selection... larger the better. I am sure some experimentation will result in great looking parts.
Gary

[tim_mcknight]

I ordered a 1/2" ballnose bit from Centurion Tools today. I will post back after I give it a try. Thanks again for helping out a noobeee.

[tim_mcknight]

Just an update... I machined 6 more fret boards today and I figured out my tooling mark and surface ripples. I used the same CMT bowl and boxx bit but I changed the step over to .020" and cutting speed to 3-ipm and they came out as smooth as silk. No sanding to do what so ever! It took about 10 minutes longer but it was worth the wait. Thanks for all of your help guys.