Hey team! I am going to attempt to carve a lithophane. I have some .332 inch thick corian but don’t have a clue about feed rate or depth of cut. Any suggestions. I am using an xcarve 1000mm, a stock spindle, 1/8" ball nose bite.
Thanks in advance,
Charley
With Corian that thick, I pocket out the back with a 1/4" end mill and leave .140" material, then turn it over and cut the Lithophane .100" total depth which leaves .04". A 1/8" ball end mill will not give very good detail. It would be better to use a 1/16" or smaller BEM. I use a 1/32" with my Lithophanes, but my spindle on my CNC router runs at 45,000 RPM. Keep your step-over distance small so the cuts will blend together. You will need to keep your feedrates down lower based on your spindle’s RPM and the size of BEM your using.
Thanks for the quick reply,
You answered my other question as to which side to carve on. As I understand you, In my case I will be cutting both. Firstly using a 1/4" endmill carve from the back side to a thickness of .140". Then carve the lithophane on the front leaving .04" of material after the carving is completed. I have a 1/16 ball nose bit that I can use so I will try that first. I assume it is best to do the entire front with the 1/16 bit or should I do the roughing pass with a 1/8 ball notes and then switch to the 1/16 ball nose for the finishing pass?
Making a lithophane is a project I have been wanting to do. What software are you using to create the toolpath?
Please let us know how it turns out.
Lets say your litho/image your engraving is 4"X6", I cut my piece of Corian 4.5"X6.5", then cut the pocket in the back 4"X6" and leave a 1/4" wall all the way around. Doing it this way, still maintains the rigidity of the Corian for clamping, but I use toe clamps from the side on my CNC router. If you need more of a wall for clamping on the top, just adjust your outer size. This gives a dark frame look around it when you back light it.
You should be able to cut .100" in one pass with a 1/16" BEM and use a .005"-.008" step-over. I use a .005" step-over with the 1/32" BEM and cut full depth with it, but I have a very high RPM spindle. Be careful with the first plunge and cutting pass from one side to the other as that will have the highest chip load and could break your small bit.
Here are two night lights I made this way.
Here is some information from John Champlain on framing and back lighting your Litho.
I think you already know, I use PicEngrave Pro 5 to engrave Lithophanes.
I was not sure if you were asking me or Charley, so I went ahead and answered you anyway.
Picengravertoo- I went with corian and followed your guidance. Love the result! After I saw that the corian was coming out really well, I went ahead and made a cedar light box. The lights I placed inside the box are a bit too dim for what I want but the result still remains awesome. This is my 16th wedding anniversary gift to my wife so I was a bit stressed that I may not achieve what I wanted to but I ended up with a better product overall! Thank you.
V/R
J.R
That came our very good Jeremy,
Thanks for sharing.
Jeff
I have upgraded my machine with a dewalt dp611. This gives me the higher rpm like you mentioned with yours. I plan to follow your suggestions about cutting from the back to leave a thickness of .140" and then cutting the litho on the front using a 1/16 or 1/32 ball nose bit. If I understood you correctly you said that you can cut the litho to the final thickness in just one pass taking away a max of .1". Can you recommend a feed rate please?
I looked at the Dewalt DWP611 and the max RPM is 27,000, so I would run the 1/16" BEM with a .007" step-over at 60-65IPM. If you use the 1/32" BEM, then a .005" stepover at 50-55IPM. This is if your cutting in white Corian which works the best for Lithophanes and it machines real nice without material building up on the cutter.
You need to set your software to cut at a 45 degree angle so it will start the first initial plunge cut in the corner and cut out at that angle from there to reduce the starting chip load on your tool bit.
After cutting a couple of Lithos, you can try increasing the feedrates some to cut down on your engraving time.
Let us know how it goes.
Thank you for the info. I will be using you suggestions without a doubt. Your willingness to share your knowledge is very much appreciated. I will let you know how it goes when I finally get to the litho carving. For now I have a backlog of orders to fill but I am making headway.
I now have a great gift to provide a great family! Unfortunately my photos do not do this project justice.
…now to solve the dust collector mystery…ha!
Thanks for the kind words Jeremy.
That Lithophane came out excellent and I’m sure they will be very pleased with your gift.
I agree, very nice work, much much better than the results I am getting. Very frustrating, I can not seem to get a handle on what is causing this. A roughing pass works fine. The depth of all the cuts seem to be correct. But switch to the Finish pass and everything goes south, way south! It starts out cutting fine but as time goes by the Z axis continues to get deeper and deeper until it not only cuts through the corian but keeps on digging into the waste board like a starving colony of super hybrid strain of termites. It has done this every time. Using Aspire to create the litho and tool paths, Setting the image height to be appox .14" with .04" material left on the back side and starting thickness of .25".
I started trying to use Universal Gcode Sender but it got freaked out with the file size for the finish pass, and so did Chilipeper. I purchase PicSender because they said that it could handle 10 million line files. I was pleased that it did not lock up at all. I don’t think the gradual increase in depth is due to Pic Sender because I had the same issue with smaller files using UGS and C-Perp. Gotta be something in the software but I’m at a loos. Any suggestions? .
Hi Charley,
It looks like your Z axis may be loosing steps. You may try decreasing the accels for the Z axis. Carving Lithophanes works the Z axis up and down quite a bit. The X&Y axis just scans back and forth. You may need to adjust the amps higher for the Z axis also.
Sounds like solid advice. I have adjusted the power to the x and y axis but never the Z. I will adjust it down then back up to find the limits and then set it at about 70% up with 50% being in the middle. My last failed attempt was using feed of 65ipm and plunge of 20ipm. Nothing looked like it was struggling but I was apparently loosing steps when z with up.
Charley,
If adjusting power does not help, disconnect the z stepper from the Z screw and check for binding by turning the screw by hand through its range. A slightly bent screw and/or a slight bearing misalignment can cause lost steps, too.
John
Thaks for the advice John, I did check that after you suggestion and am happy to report that the Z was smooth as butter. Turns out the Z stepper just needed about 1/8 of a turn of the pot to bump up the power to it. Worked fine going down but just didn’t have enough umph to raise it all the way so it was loosing a tiny tiny bit. Over thousands of ups and downs, missed steps moving up compounded to become a major problem. Thanks to your suggestion though, I know that I don’t have an problem with the screw or bearings.
