[Stewey]

HI Folks, this was a first time lithophane for me, and it worked well, I reckon.
(The 2nd time one had a few problems though...!)

It was done for a Christmas present for an uncle who's 93 years old. It's of a photo of his parents in about 1946, with a grandson of theirs.

It was done in 3mm opal perspex-type stuff whose name I've suddenly forgotten, and is 21 x 29 cm.

The three photos show it close-up half roughed with a 1/8 ballnose endmill & half cleaned up with the 1/16" one, then the finished product, then the finished product held up to the light outside, so it doesn't look like a negative anymore.

Regards, Ian

[bill south]

Nice Job Ian;
What software did you use to generate your code? I'm assuming that you started with an old B&W photograph.
I'm sure Bill was quite pleased with your work.
Bill

[Stewey]

Hi Bill,
thanks-Uncle Bill loved it- and yes, it was from an old B&W photo.
We use enroute3 software. It came with the router when we bought it. It has a dongle too, so you can't swap systems, without shifting the dongle across.

[tjskcnc]

Hi~
Beautiful work.
Please post more detail.
This section of the forum is for "tips and tricks." Basically, how-to's on creating different projects, not just posting images of finished projects.
I do not have the same software as you, but would like to know the complete process of how you created this piece, such as material prep, material used, possibly material resources for hard to find materials, process used to convert images to actual usable machine code, etc.
I have signs all over the western states, but you can find much better work than mine in magazines such as Signcraft and Signs of the Times, even links to sites from other sign makers here. Unfortunately, they do not detail processes in creating them.
I am not criticizing your work (which is very good.) There are a lot of people like me that are extremely busy and do not have as much time to experiment as others, but would honestly like to know HOW you got to the final results, and see how we can apply them to our own work.

Thanks for posting. Please continue to do so. I love seeing lithopane projects and plan on trying my hand at it very soon.

[Stewey]

HI TJSK,
I know what you mean about finding time for 'experimenting' hence it happened at Christmas time, at the last minute, when we needed/wanted something nice for a relative who didn't really need anything, etc etc. There was a storm brewing in the distance, and the elderly uncle was due to arrive within a couple of hours- no time to spare but the 'present'.

The steps followed, in order, (including errors), were:

1. decide to do it- i.e. something, and to finish it.

2. find a nice photo, preferably with a good range of grey shades, and a few hard edges.

3. open the photo in Photoshop or other image editor, and adjust the levels, or amount of black or white, to achieve a nice scale or range from light to dark. You don't want it to mostly all be light, or all dark, for instance.

4. size it to suit the material thay you've just found. I had some samples of this stuff from a Letterheads event in Australia. It's a plexiglass/perspex/acrylic type of product made by Bayer. I had a few sheets of 21 x 29 cm x 3mm thick (just under 1/8").

5. convert the picture to greyscale- this should have been done earlier actually. When finished, sharpen the picture a little, and save it as a jpg.

6.I screwed the sheeting to the MDF spoilboard, with drywall screws around each edge- just the countersunk heads hold it down, and the shank prevents movement.

7. I put a 1/8" ballnose tungsten endmill in the router, for a roughing cut.

8. Back to the software- with enroute, you define the plate- in this case 210 x 280 x 3 mm, and with a blank plate you import the jpg file of the photo.

9. to make it a relief, you draw a rectangle the size it's going to be, allowing for a suitable margin (about 2" on all sides here). Then convert that 2D rectangle to a 3D relief with the 'make relief' button- give it a height of zero, a flat top, and a resolution of 100 dpi. You now have a photo-sized 3D relief of zero height/thickness.
Centre it where you wish, allowing for the margins to be equal, or a whisker more margin underneath it, for a nice appearance.
I drag guidelines it to each edge to help. Othertimes, I'll draw a big box the size of the whole plate, and select all, and centre all, then delete the big box. Other times I'll creat guidelines in the dead centre horizontally & vertically, and use those to align the relief's 'handles' with.

11. Position the photo over the relief, and select the 'apply bitmap to relief' button.
It'll ask you which relief to apply it to, and what overall thickness it's to become. I chose 2.35mm- that'll allow for 0.7 mm of material in the thinnest parts, plus allow for inaccuracies in bed thickness.

10. Take the photo, and OOPS- the relief is going to be high on the white bits, and deep in the blacks- and that's the opposite of the effect you want with a lithophane, so quickly reopen your image editing program and open the last saved picture and invert it to make it a negative and resave it.

11. Go back to the relief and use control-Z or undo, or the 'delete relief' button, and redraw your flat rectangle & make it a relief of zero height again- it's all good practice!
Now you're glad you drew in those guidelines- it's easy to realign the new relief where you want it on the material plate, if the 'snap to guidelines' option is turned on.

12. Import the negative of the photo, position it over the relief, and choose the 'apply bitmap to relief' button once again, tell it which relief, and set the thickness it's to become. Press 'enter' or 'apply' to get it all done.

13. The relief will be sitting in the air above the material plate, so use the button which says 'align all reliefs to the top of the plate'. This pushes it all down to sit just touching the inside top surface of the material, and leaves a skinny bit of untouched material between the bottom of where the lithophane will end, and the bottom of the material.

14. Save it. The you need to apply a toolpath, Enroute does all the 'post processing' to create the G code, as well as being a design program. So, select the relief, and I chose 'hatch fill' of the toolpath options. That opens a tool selecting menu, where you set the 1/8" endmill, I chose the depth to be 2.35mm full depth of the file, but allow this tool to stay 0.8mm off the bottom of the cut. Overlap was set for 60%, and speeds were- well I tried 130mm/sec for X & Y, and 30 mm/sec for Z, but it trundled along quite slowly except where it wasn't changing height much. If I reset it to 80 mm/s X & Y, and 20mm/s for Z, it still went no more slowly & no faster. There's a limiting factor somewhere in Z that I'm not aware of. Y only moves a whisker per pass- just the 60% OF THE 1/8" TOOL DIAMETER oops sorry about the caps. X speeds along smartly when Z isn't changing. Must be somethng somewhere that needs editing- no idea where. (The Z axis servo did get awfully hot though, duting the 1/16" cuts.)

Anyhow, it took maybe 18-20 mins to rough it out with the 1/8" endmill after I'd exported the G-code & saved it.

15. I then edited the toolpath, to be run with a 1/16" diam ballnose endmill, at the same speed, and 66% pass overlap, and full 2.35mm depth, and checked it all by looking at the perspective view to ensure it was moving up and down, not just flat bottoming the whole picture out (yes, I did that with another file once, not a lithophane, but I ended up with a big oval empty space in a lovely bit of timber...) Actually you need to verify the toolpaths look right, back when you create them with the 1/8" ballmill in step 14.

16. Change cutters, put the 1/16" ballnose endmill in, sense the tool length, and start routing. It took about 1 3/4 hours to do the rest. We had a lightning strike in way out the distance which caused a flicker of mains power, the PC & the onboard computer in the router kept going, but the rotary 3-phase converter powering the spindle died. The cutter started to drag across the material- quick hit the emergency stop!

17. Restart the file- oh, no, not an hour and a quarter of waiting to catch up to where it left off...what other options are there...thinking thinking...

a. I tried this once- 'guillotine off' the part of the relief already done, using the 'subtract from relief' option after making a new relief as a box over the part you want removed- and export new toolpaths. Sounds great, but it made the toolpaths go at zero height (plate bottom) over the already cut stuff, ruining it, in a former attempt at being a genius, so that won't work.

b. similar idea- only ADD a flat topped box to the file, and merge the highest parts. That did work- it skipped quickly over the parts at high speed, taking about 15 mins to get to where we had to pick up from, saving an hour's wait.

c. Thinking later, in hindsight, I should have just rotated the piece (the relief)180 degrees, in the program, generated a new toolpath which now starts at what would have been the end, then rotate the piece/relief back 180 degrees to where it was, and export that toolpath to G-code. That would make the file start at the other end and work its way through up to where it ran out of juice the first time. You just stop it then, after they join up & overlap, hoping like mad that you didn't accidentally move the relief a mm of so in your rotating. (Hence using guides & the 'snap to' option)

Ordinarily, it'll rotate around the dead centre & rotate back without being displaced, so there's no problem, but it's easy to get carried away & accidentally move something a whisker. Be careful!

18. In this case, I added a black outline and then a white outline to the original photo, before saving it. IN hindsight, I should have just created a single perimeter 'frame' and routed a groove in/around that, as an entirely separate 2D offset toolpath, once the lithophane was done. I did that afterwards anyway, to neaten up the edges of the deep 'white' groove previously created.

19. Decide on the text, the font & size, and I appllied it as a 2.5D vee-grooved or engraved toolpath with a conic or 45 degree engraving tool. It was one of those tngsten engraving cutters which is sharpened by being half flat across the diameter. It wasn't a good choice of tool. It was brand new, but the plasticky bits just reglued themselves to the material after being cut. Maybe I should have run the router faster & the spindle more slowly...? So, I ran the text cutting G-code a second time, and that cleaned out the gunk better, and a nail-scrubbing brush followed by an exacto knife blade dragged on edge did the rest of the furry bits.

20. Unscrew the material from the router bed, vacuum up any scraps of plastic, and go outside to look at it with the sky as the background. Congratulate yourself that the tool didn't go right through to the spoilboard in any places, and that the 2nd pass to finish it after the power failure linked up almost imperceptibly with the first part.

The effect is that the material, opal or milky-white ( I've just remembered, I think it's called Makrolon, or Makron or something like that)- the material is thinnest where the picture is whitest- allowing the most light through from the back. The material is thickest where the picture is blackest, filtering out most of the light. In between are lovely gradients of appropriate grey.

It looks like magic comparing the fuzzy queer looking front, with the proper image when back-lit.

This was the first time I tried to do this so I'm no expert. I did consider starting with a greater overlap- say 85% per pass with the 1/16 cutter, but it would have taken forever, and the detail just wasn't in the original photo to be preserved with a 1/16" cutter, so 66% was quite OK in my mind. Maybe 50% would have been tolerable also, I don't know.

Our router sometimes doesn't do its heights properly. I have no idea why. When I ran the first file, the 1/8" one, I told the machine that the material was 3.6mm thick above the bed, not 3mm, just to see how the paths started off- I didn't want it scratching too deep in places where I had no grace. After it looked OK, I restarted the file with the overall thickness set at 3.15mm, even though the stuff was 3.0 thick. I left the file set at 3.15, and I'm glad I did.

Another piece of advice- use a clean sharp (new) 1/16" endmill to cut the plastic stuff, not an old worn dirty one.

I tried a second file a day later, making it from an oval relief. It would have worked but the storm brewing did it's trick with the power again when I wasn't babysitting the machine, and it started to gouge the piece where I didn't want it to, onluy it didn't lift at all, so we had some zero height gouges. I tried to rerun the file later, but in my imnpatientness (?) to save a lot of time, I ended up toolpathing the wrong bits, and gouging away the background that was supposed to stay untouched. (In haste, I didn't check the toolpaths in perspective view before exporting them to G-code, you see... Pride comes before fall, or several falls, and very much so...!

So...I hope that helps, or at least, is somewhat entertaining!
I am sure there would be equivalent processes in other software.
Enroute came with the machine when we bought it, and I don't mind it. It's not the newest version. I'd like to get that one day, after I get the bugs ironed out of the machine, and it's paid for itself, first. Aspire also interests me- I'm uncertain how they compare in terms of what they can do, or their limitations, except that the price difference favours Aspire.

There was no material prep except removing the plastic protective sheeting. I thought about framing or boxing it up & backlighting it, but it was fine as it was. It'll be a good talking point for him in the retirement village he lives in. He loved it!

[Stewey]

Oops, double-post, sorry!

[tjskcnc]

Hi Stewey~
Great "T'n'T" response. I think every one can learn more from your 'mistakes' than what you did correctly.
Thanks again.

[Stewey]

Thanks- I hope so!

It'd be nice if others posted their summaried or differences of attempts, too!

(P.S. what router design software do you use, and have you any experience tuning the PID variables? I need to get the heat out of the Z servo& am guessing one of the parameters may be incorrect.)

[mactec54]

Hi Stewey

Nice job on the lithopane & your post on how to do it.

For your PID tuning you should ask that in another post just by Its self, Most will just be looking at your lithopane so it may not get noticed

[Stewey]

Thanks- I know that (re the PID tuning query) I was just interested in TJSK's opinion or experiences, that's all!

[tjskcnc]

Hi~
My list of software:

Solidworks 2009
Mastercam X3
Alibre w/AlibreCam
Ucancam v8
Vectric Cut2D
Vectric PhotoVCarve
CabinetsPartsPro
Cambam
FreeMill
NCPlot

Graphic Software~
Adobe Illustrator
Adobe Photoshop
Inkscape
Gimp2
Micrografx Photomagic and Windows Draw (simple and awesome programs, but they were eventually bought out by Corel)

And a bunch of other miscellaneous Cad/Cam and graphic stuff that doesn't get used much. Most of what I do can be done in with the Vectric software, Micrografx, Adobe, and then processed for Mach3.

Inkscape has a very good Trace Bitmap function in the Paths menu that is excellent for tracing images for converting to vector graphics, such as dxf or eps. It's also free (for now). They also have a great help site with detailed tutorials.

I also use DeskEngrave and Stick Font, two more excellent CNC lettering programs that are (for now) free.

Google searches should find them easily.

You should get these programs while they are still free.