Lithophane problem

[brian]

Just did a second pass on my first lithophane.After the first pass(.125 bit.0250 setover 2IPS at 15000rpm)it looked pretty good but room for improvement.Did a second pass reduced the setover to .010 and Z to -.005.The finished product looked fuzzy.On the first pass the finish was smooth on the second it was rougher.The best way to describe this is its like the difference between a 120 grit finish VS a 600 finish.
The only thing I changed was the bit.I was given a new bit a .125 round nose CMT.The previous bit was a Freud bit.
Could it simply be the bit or could the machine have lost a step or two making it blurry.I took a wet rag and wet it down and it was quite a bit clearer till it dried.
By the way I used a cream coloured corian.

Brian

[brian]

Just had another thought could the stepover be to small for this type of material

Brian

[billp]

You can take your stepover down to 5% if you have the time for a long cut. Guys have gone down below a 1/32" bit diameter in Corian, but only for highly detailed stuff.
You don't mention how you are holding the Corian down for your cuts. Vacumm works the best. Edge fastening can cause a "diaphragm flutter" in the center. Since you got one good pass is it possible you moved the piece between cuts while wetting it down? Are the bit geometries different? ( number of edges, angle of rake, etc). Corian isn't bad on bits so you should be able to try another version with the second bit, and a low stepover, and see where the problem is.

[harold_weber]

Bill, from my notes taken at the 2006 ShopBOT Jamboree, Scott Feimster (the speaker from Onsrud) said that if you take too light a cut in plastic, the finish will get worse. He recommended never taking a cut less than 0.015 with an 1/8 inch bit. I have used .0125 stepover and 1/8 inch bit on Corian with no problems, so is Corian an exception to Feimster's rule??

Brian, here's a vacuum fixture I use for lithophanes, its made from 1 inch thick HDPE and Allstar "inboard" gasketing. Grooves are .25 inch wide by 3/16 inch deep. The fitting at the bottom is an old tire valve stem pressed into the cross-drilled hole.

6896

[billp]

Harold,
Since Corian is not a plastic per se I would think that the rules might be different. I've used the smaller stepovers in the past with no apparent degradation of cut quality.

[Brady Watson]

Harold,
The '.015 rule' is for 2D profile cutting using o-flute geometries only. The shoulder behind the cutting edge on o-flute bits, designed for plastic, fall away abruptly to minimize rubbing & heat. Without an adequate chipload, the cutting edge can't consistently 'dig into' the work. It does not apply to a ball end mill in 3D. Totally different geometry, cutting direction & forces between the 2.

-B

[harold_weber]

Brady, where did you get this information? I have not noticed it in any Onsrud literature.

[Brady Watson]

Harold,
I have the special teacher's edition of the Onsrud manual with all the answers in it...you mean you didn't get one?


Don't believe everything you read in books, nor discount that which isn't written in a book...the best learning comes from doing, not reading. If you go off of the values suggested in the Van Niser articles on plasticrouting.com , they say, "Without at least .015"-.030" of material to remove, most acrylic router bits will not have enough material to bite into and will actually show a deteriorated finished edge over the initial roughing cut." The article by the way, is about premium finishes in acrylic with a focus on 2D profile cutting. Nowhere do they mention 3D or ball end mills. Only your own research & testing will fill in the gaps when it applies to 3D milling.

You are simply not going to remove .015 to .030" in acrylic or solid surface with a 1/16 or 1/32" ball without snapping off the tip. Furthermore, if you ran a stepover of .015 with a bit smaller than .125" dia, it's not going to look good since it will show distinct stepover marks...Personally I would 'rough' out a lithophane with an 1/8" ball using a regular 3D raster strategy and .003 to .005" allowance. Then finish with 1/16" or 1/32" bit depending on the level of detail I wanted to achieve.

-B

[harold_weber]

Ahh, the Van Niser Articles... I tried their polycarbonate recommendations when I first got my machine (the current software was Version 2.29). The results were very disappointing and that's being kind. I was able to IMPROVE the surface finish using 36 grid sandpaper. But that was 4 years ago and now with a stiffer table and gantry, Perske spindles, finer step capability, and the latest "smoother" Version 3.5.0 software, I'd better go back and have another look at this information.

Thanks Brady.

[brian]

Thanks for all the replys
Just ran the same program(same setover speed etc.)
The only thing I changed was the bit,I used the same bit I originally used a Freud .125 round nose.I took another .003 of the same project and it fixed the problem.
Both were new bits.The CMT being more expensive gave a worse finish than the cheaper Freud.I don't know if this would be the same on wood.I'll have to compare both bits on various materials.I know bits vary but you'd think a so called better quality bit would give a finer finish.
Any thoughts on this.

Thanks Brian

[Brady Watson]

Harold,
Even the glorious 'Van Niser' articles I find fault with...I just listen to what the machine tells me as I adjust speeds & RPM as it cuts. I never adhere to advertised chiploads since 99.99% of the time they are completely wrong...one wonders how they get their data...Incidentally I cut some 1/4" acrylic last night & found that I was getting beautiful edges by stepping down the bit only .0625 per pass and moving at 2 IPS. I think I was spinning about 14 or 15k on the router. Normally I would do a cleanup pass with allowance, but I saw no waterline marks or anything...I was taken back by the fact by this, plus the fact that the edges looked like they were sanded with 220 grit paper and nearly ready for flame polishing. I have to cut some 3/4" next week so I'll see if it applies to that as well. I used a double O-flute (1/4") for the 1/4" stuff...I have a fresh 3/8" for the thicker stuff.

Brian,
I would steer clear from using router bits for doing 3D. I would try to use end mills as much as possible. They are solid carbide, cheaper and ALWAYS dead on advertised diameter...I can't say that is the case with any particular brand of router bits. They all seem to vary. Plus, end mills are like upcut spiral bits and pull the chips away from the surface. The only 'router bit' that I would recommend is the one that comes in the starter kit that SB sells. It is a 1/4" shank tapered down to a 1/8" ball. (these are also made by other manufacturers as well. I get them for about $30 each)

-B