That's right!:banana:
I cut this 10"x12.5" (actual cut area) Lithophane without a roughing toolpath on .25" corian using a 45 degree V-bit!
I took the picture of this huge sculpture/waterfall at the Jackson Rancheria Casino in Jackson California yesterday.
I have attached the PhotoVCarve cutting parameters page, as you can see I told the software that I am using a 0.031 ball nose bit.
I set the Z zero at -0.1" and cut it in one pass.
Cutting at a 45 degree angle is essential with this method as it is a deep cut.
With the V-bit once the first pass is cut each subsequent pass is only shaving the edge of the previous pass.
This is why the roughing pass is not needed.

Bill Schober
Pine Grove, CA

bsimages

Nice Image and great result. Looks like I'm going to have to add PhotoVCarve to my list.

thanks for posting

mind if we sak feed rate and cutting time?

Look at the second image for the cutting parameters.
It took 16 hours but I cut it slow (30/30 inch per minute) as a test to watch the cutting and make sure it was working ok.
Bill

Great job Bill,
I love it when people come up with better ways and share thank you very much. :)

I asked http://www.centuriontools.com/index.html?cart=118633447063440298 about 20 deg v-bit and 45 degree so far this is what they said about it.

The only thing close to what you are looking for is a 30 deg v-carve bit 1/2" diameter. We don't have these in 1/4" at this time. 20 deg would be too shallow an angle, the tip would not have a lot of strength. The other option would be an engraving bit, we do not have any on the site yet, but will in the near future

I order bits from them week or so ago. look great, havnt tried them yet.
I am sure they will work great from what others have said. Good prices too.
I will be ordering 30deg to see how it works

Thanks Again Bill

Kent

Opps double post please delete thank you

Great let me know how well it works!

Bill

Hi Bill,

Great Machining Technique and Thanks for sharing the idea!

Running a roughing toolpath when working with thick material / corian is always a major hurdle for new users. This approach makes it much easier to understand and potentially quicker to cut.

Fantastic Lithophane too!

Tony

Thanks Tony,
I just cut one at 50/30 (50 inch per minute on the X&Y and 30 on the Z axis) and it came out perfect and took 7 hours and 28 minutes for a complex 10"x12" lithophane...next attempt will be 60/30!
Bill

OK bill that was just mean !! NO Picture:confused: . I can't wait to get my bit and give this a try .

Used a cheap 90 degree V cutter on 3mm White Perspex to see how my DIY machine would handle it. Cut depth was 2mm but everything else very similar to yours Bill. Feed speed 1750mm/min machine time approx 4 hours. Pleased with this first atempt but definatly need something less than 90degrees to get rid of the halo effect. Anyone tried a litho in transparent sheet and lit along the edge(like a fibre optic)?

Thanks for the tip Bill. I notice on your lithophane you have a neat border where their is detail. How do you do it?

I get the nice neat border because I am using 1/4 inch corian so my Z zero is a 1/10" below actual zero...with a max cutting depth of 1/10" it leaves the lightest areas at -2/10" and the darkest at -1/10 and the uncut area at 0 hence the nice neat border.
Was that clear as...as mud?
Black&Decker sells router bits with 45/60 degree V-bits on each end for under $5. It is what I have been using.

Bill

I've been using 1/2" corian so I have to rough it down to 1/4" thickness before running the litho program. By cutting a pocket 1/4" deep, I wind up with a frame. The advantage is there's something to clamp to while running the litho.

http://mc-machine.com/crokes_pics/v/lithopanes/

Oh yes the other thing I did was to place an x in the center of the corian and used that as my X & Y zeros thus leaving an even border around the outside of the piece. Of course you need to square your material on your CNC machine. And tell the software that you using the center as your zero which is as easy as a mouse click in the "Set material size" page of PhotoVCarve.

Bill

I get the nice neat border because I am using 1/4 inch corian so my Z zero is a 1/10" below actual zero...with a max cutting depth of 1/10" it leaves the lightest areas at -2/10" and the darkest at -1/10 and the uncut area at 0 hence the nice neat border.
Was that clear as...as mud?
Black&Decker sells router bits with 45/60 degree V-bits on each end for under $5. It is what I have been using.

Bill

Crystal clear. Thanks Bill.

Nice work -

One problem I have noticed, using a V-Bit to cut a Lithophane, is it leaves some artifacts behind, diagonal lines and black specs, when viewed with back light. If you use a scrub brush with soap and water, allow to dry. Then simply apply a coat of clear spray lacquer, you will not believe your eyes!

Bill Schober
Pine Grove, CA

Hi Bill,

So the second is unscrubed and the third is scrubbed them lacquered, I would have to say that its a huge difference for such a simple idea.

Good work

Sean

Any links to where you purchase the material from?

Which material? The Corian? E-Bay. The clear lacquer? Wall Mart ($0.98).
Bill

Great idea about the scrubbing brush and Lacquer. I can't believe the difference. In the past I have washed the finished image with soap and water to clean and then applied a smear vegetable oil to give it a glossy look and blend any perspex that had gone white but your idea sounds much better.
Your use of center is brilliant. I always spend ages trying to line it up when it was so simple all the time.
I will give these a go next time. :)

Cheers
Peter

What is the best program for cutting litho's. I am new to the CNC world and would like to start cutting lithos. I have done some photoengraving with image carve, but am unsure if it will work for lithos.

Thanks,

PhotoVCave from www.Vectric.com , they even have a FREE trial version. They have tutorial which makes it easy to try.
Bill

Bill,
Where do you get your bits? You mention Black and Decker, do you have an online supplier?

Another way to get a even frame is to mill a rectangle around the main image, leaving .125" stock (or whatever frame width is desired) between the image and the groove.

I mill my grooves .150" deep in .250" stock.

I then use a bandsaw to rough the piece out of the larger stock, cutting down the center of the groove. Then I use a disk sander to smooth the rough edge.

bsimages, did you wash and laquer the eagle picture, or is it finished in some other way?

I scrubbed it with a stiff nylon bristle brush and dish soap. I then gave it a clear coat of lacquer. I have since discovered that if I set the depth to 0.15" in PhotoVCarve and then when I cut it out, I set the Z zero at -0.05". I get more of a 3D effect in the Lithophane. This gives 50% more depth than the original method of setting the depth at 0.1" and the Z zero at -0.1". Not only is there more depth but also the for potential more shades of gray.
Bill

I had an interesting thing happen. I have been using a 40 degree included angle engraving tool with a 0.010" flat on the end. I get better detail than my 0.032" ball, but a lot of remelt. The customer asked my to decrease the total machining range to lighten up the lithopane, so I cut it from .100" to .050".

No more remelt, and the finish was much better.