I have been asked to carve a world map.
I have a file but not sure what are the best tool paths to get the most detail.
I plan on a final size of about 12 x 20 x 1.75
here is a picture of the (hopefully) final product.
I have been asked to carve a world map.
Roughing toolpath with 1`/4" end mill. Finish toolpath with a .032 radius tapered ball nose bit.
OK so I am getting closer to starting this.
I’m starting with a 1/4 endmill.
would it be better to use two different bits for the finishing pass.
Thinking of using a 1/8 flat endmill then switching to a 1/32 ballnose for the final pass.
Would I save time without compromising the detail, if I increased my jerk settings to 8000?
Also would the finished project look better is I did my finish pass on a 45deg raster?
Any other steps to shorten the carve time?
Where did you get the file from?
It was purchased from Etsy.
Logo in picture shows what Etsy shop.
I tried to look it up with that but will try harder.
Thanks, Looking forward to see the final project, very cool
Well my first try was a failure.
here is a small corner of what the model should look like.
Here is a picture of what I ended up with.
Not at all pleased with this result.
I would like to know if anyone has any Ideas on how I should set my toolpaths to achieve an acceptable result.
I have a 1/4 end mill for my roughing pass.
I have two different bits for my finishing pass, 1/8 endmill for clearing and (my problem?) a 1/32" tapered ballnose for final.
It seems like the 1/32 ballnose if poking holes all around the edges of the "camel and the female in the corner.
I did notice that when importing the STL file, and converting it to inches, the original was 3 times as large as my material (x=31 y=19).
I am wondering if there are some STL models that just don’t carve well.
I have sent a message to the etsy shop to see if they have even carved this.
If I can get the right toolpaths figured out I think I can “lower” the model say 1/16 of an inch and run the finishing pass again?
here is my finishing pass settings:
And my 1/32 bit settings
My material is teak 31x19, and my Z is set to the machine surface.
This is my most detailed 3D carve yet and I expect to learn from it, but I would like a nice finished product.
I can supply my CRV file if anyone wants to take a look.
I would also share the STL file for troubleshooting purposes only.
Thank you for looking at this.
I recently carved this (box still a work in progress so I can’t show the finished version I am making for a friend).
1/16"R in progress on right side, with what the roughing did on left side.
this is the final carve followed by 300 grit sanding wheel across surface…it takes out a little detail but gets rid of all the fuzzies. Lighting does not really show the detail in picture…there is more detail on leaf surfaces and whatever those little berry/bud things are called.
My recipe for this carve in cherry:
- 1/4" upcut whiteside bit, 19000 RPM, .006 inch feed per tooth for 228 IPM feed, 114 IPM plunge feed, with an 3D adaptive tool path. I leave .02 inch stock both radially and axially,
- 1/16" radius tapered ball nose from Spetool, 18000 RPM, .008 inch feed per tooth for 288 IPM feed and 180 IPM plunge feed, using a 45 degree to grain parallel path, no stock to leave, 0.25 * bit diameter (.029356 per fusion)
- .25mm radius tapered ball nose from Spetool, 18000 RPM, .005 inch feed per tooth for 180 IPM and 144 IPM plunge, on a -45 degree to grain (that is to say 90 degrees from the other ball nose) parallel path, no stock to leave, 0.27 * bit diameter stopover (.00485323" according to Fusion). I stepped it up from test at 0.15diameter which took forever with slightly better results and down from 0.3dia which left noticeable tool marks)
I use Fusion 360 and don’t know what control you have over tool paths in vectric (or is that carvco?) I typically specify feed per tooth and let F360 calculate feeds since it is a better thought process for me to adjust that for a given bit and wood. On a 3D carve after roughing to .02" material, the bigger ball nose is more limited by how fast the onefinity can change Z direction than by the bit limitation in material. Ditto for the small ball nose after the bigger one runs. Also, I took advantage of PWNCNC Yellow Friday (Memorial Day sale) and upgraded to a 2.2kW water cooled spindle a couple of months ago. If I was still using the Makita, I might go a little easier on the 1/4" bit for roughing…use whatever works for you already since it does not appear the roughing is giving you problems. The ball nose feeds and speeds are well within the Makita’s ability.
How much control does your CAM software give you over each tool path? Can you set parallel paths and specify direction?
Mine was an Etsy stl too. Fusion complained about it not being water tight. I had to make it water tight, which was a bit of a pain and required reducing detail by about 20% to keep fusion from taking forever to calculate how to make it water tight.
The roses are about 9"x5". It took 4 hours to carve with the .25mmR. I don’t recall how long the others were, but probably close to another hour for both 1/4" and 1/16"R
Also, I zero off a 1-2-3 block and not the wood after aligning to an L bracket that I carved parallel to both X and Y that is fixed to the table. For more detail, I put one 1-2-3 block agains the X arm, and another on the Y arm, then fix the wood to the spoil board. Any time I Z zero a bit, I do it from the corner of one of the 1-2-3 blocks. I return to zero between cuts so my XY zero are preserved even if I shut off power. I broke the 4 hour .25mm carves into 1 hour(ish) blocks and was able to run over several days and power offs with no issues.
Hope that helps n good luck!
After seeing your post, I bought the same file on etsy, I plan on a test carve in maple before doing one in Walnut, very interested to see what Etsy has to say to you.
Please let me know.
your project is very challenging. Yet, I have no experience with such detail. But I would always try ball nose bits for the final pass. On hardwoods, you can get a nearly polished finish with those ball nose bits:
Catetory Radius Mills
Well after several messages to the Etsy seller I was disappointed.
it took three tries to get the seller to admit that they haven’t carved this model.
The seller told me that all her models use the same bits.
to quote her:
“Im telling you the right tools to use for all models, we have our softwares in mm soo, for the finishing pass, 0.5mm 10° V-tool, toolpath 0.25mm”
she also included this one picture.
In my limited search this seems to point to this website:
the model may be good but the seller isn’t very knowledgeable (seems to me)
Hi Mitch thanks for responding.
My CAM software is vectric Vcarve pro version 11.506
vectric will allow me to set multiple tools for the finishing pass, and I believe I could set different direction for each (I have not done that)
I’m not familiar with Fusion what does it mean to be “water tight”
Also have you run into STL files that you won’t carve because of the detail?
I’m wondering if there are some files that are not meant for CNC carving, but 3D printing?
A .25mm radius bit is even smaller than my 1/32 diameter (.0156R) it is no wonder that it took 4hrs on 9"X5" roses.
What do you think about being able to salvage this project by moving the model 1/16 lower in my CAM software (vectric), then setting up a slightly different tool path strategy. My concern is that I would loose the ultra fine detail.
One other thing how do you break the 4hr .25mm carve into 1hour blocks, and is that something that can be done in vectric?
I’ve carved a few models similar to this, though not this particular one. Your result looks to me like some of the ones I’d had, early on, when not using my touch plate to set the z height. It’s definitely needed for stuff with real fine detail.
To break up the carve using VCarve or Aspire, draw some rectangles over the model in the software. Create toolpaths that will carve within the boundary of the rectangles. Not at my laptop right now, so I cant give more detailed instructions at the moment.
Edit: At my laptop now. Here’s a quick walkthrough of breaking up the finish paths for Vectric software. I’m using Aspire, but VCarve is the same software with a reduced modeling section, and this will also work there.
Draw some rectangles around the model. Use node editing mode (press ‘N’ on keyboard) to modify the shape of the rectangles so that they’re close to the shape of the model boundary.
Run the roughing pass as you normally would, ignoring the boundaries you just created.
For the finishing path, select the model and one of the boundary rectangles. Use the “selected vectors” option in the machining setup. Make a finishing path for each of the boundaries you created.
Run one of your finishing toolpaths and see the results.
I will be messing around with this this week and let you know how it works out, the pic in the sales ad looks very good and I hope to repeat that.
Water tight is when a solid 3d model has all triangle mesh with a surface normal outside the structure and an enclosing volume without holes. This creates and inside and an outside. The stl I got had not bottom so it was a two dimensional shell that enclosed no volume, sort of like one side of a sheet of paper with no thickness. Additionally, there must have been small triangles missing from the mesh too because of the calculation times f360 was taking to repair it.
Changing it in CAM may not work since it will be working from a new relative offset, what might work is setting the Z zero some amount lower that wherever you are measuring, like the 1/16” you said. You might salvage the wood that way. I don’t think you’ll lose detail as long as you don’t shift the piece, that is just lower your measured zero by whatever amount will guarantee all current surface is recut. Have you figured out what is causing it to look like that? I wouldn’t lower measured z until you know you’ve accounted for whatever caused it to look different than the model.
As for some for printing and some for carving, as long as your CAD package can read the file and you can slice or CAM it, it should be makeable at whatever detail the respective devices support.
I break up the model by drawing a bounding box around the various pieces (with some overlap to ensure smooth transition) and constrain the tool patch inside it. Fusion CAM has several tabs. One deals with geometries which allows selection of model, exclusion of hold downs, constraints, stock models, etc.
Thanks Dan for the detailed instructions to break this up into smaller groups.
Yes I do use my touch plate for setting my Z,
I have it set to my machine base so should be able set my Z height.
I’m curious about the model you showed, (looks similar to mine) did you get the fine detail you wanted.
what did you use for your finish pass (bits)
It came out pretty good. Didn’t even really need to be sanded. Honestly, I should have probably used a finer tipped bit, as some of the fine details (numbering on clock dial, for example) were lost. I believe I was using one of the tapered Jenny bits, but it’s been 2 years.
Adding my response here as well for completeness:
I would recommend viewing the STL in something like Meshmixer. It has tools to detect issues such as open paths, “water tightness”, etc. Even something like Prusa Slicer can repair STLs as well. Without seeing the file, I can’t say for sure if that’s an issue. As mentioned, a 1/8" ball end mill (2 or 3 flutes) or a 1/16" end mill should work for finishing. Smaller just means more time finishing. Hope this helps.
I am just finishing the World Map in Cherry as a test, I used a 1/4" Flat endmill to rough and 1/32 Ball nose tapered end mill to finish.
13 Hour carve for the finish, it looks pretty good and little to no sanding, i will post a pic today or tomorrow.
I did get two files, one for 3D printing and one for machining, the machine file is huge the 3D print very small.
I used a .003 step over for the finish carve, pretty slow but good detail.