Hi, I am needing advice as to the best solution to CNC an embossing die using my C Beam. I am trying to CNC an embossing die and have some difficulty in translating a sketchup model into a gcode file. Using the Phlatboyz plugin, I am using it to define the cut parameters both inside and out but am having issues on how to remove the material that remains outside of the design boundary. What other software besides Sketchup would be recommended? I am trying to find open sourced solutions. Thanks.
Thanks, downloaded the trial version and exploring it. What flavour of gcode do you output the Vcarve paths to when cutting? Don't seem to find the c beam option listed.
Assuming you are creating designs that stand a few mm above the surrounding material, I think you might be able to use F-Engrave. It can take a B&W image bitmap and carve it out. It can do inside or outside carving. Best of all, it's free. I have used it quite a bit and am still amazed how good it is for a free application. you should select GRBL post processing.
I would use the pocket tool. If you post your sketchup file here I will show you how... maybe this will give you some ideas...
Am planning on cutting a die for use with a heat embossing rig, the material I will be using will be brass with a M5 hole for use with a M5 bolt. The F Engrave seems interesting. I have tried the SketchUCam solution but am encountering some problems in removing the face material from the desired artwork. Am doing this for the missus leather designs.
In the video I referenced I do exactly that operation, I removed the face material around that central hub. Consider the central hub to be your text, then removing the face material is the same operation and the same technique can be used to do it.
Thanks for the tip. I guess, i was trying to figure out how to mill the text directly on the brass media. My idea was to model the brass block and center the graphic dead centre. I got the text outer and inner paths defined but am stuck on trying to define the paths that allows me to pocket cut the surrounding material. Everytime I move the text element into the block defined for the text to sit on, I lose the ability to define the pocket tool paths.
I've never gotten sketchucam to do letters or freeform images very easily. Pocketing has problems with complex irregular shapes. F-Engrave, however, is simple for this and works pretty well. See the attached screenshot. The yellow, red and crosshatched areas are tool paths using different ways to carve away everything that wasn't the letters. By the way, 100mm high is probably way bigger than you would want. There's an inlay tutorial on the F-Engrave site that will show you what to do. Just use the prismatic part.
I just tried it with a simple circle and a word. so long as the bit (0.5mm in my case) can fit between the letters the pocketting will 'just work'. I had to move the S's apart a little to ensure a gap of 0.6mm so the bit can fit. of course the word must be exploded, as described in this video . A quick read of the help for the pocketing tool will also help because this needs a FLOOD pocket where you 0 - make sure the letters are exploded and each one has a face 1 - select the tool, 2 - press 'home' to go into flood mode, 3 - hold CTRL and click so it inserts the outlines (hover over the face of course) 4 - release CTRL and move the mouse slightly to redraw the zigzags, and click. 5 - press spacebar to get out of pocket mode (this is just convenience, the zigzag gets recalculated and redrawn for every mouse move so for very small bits it will appear to have hung, move the mouse as little as possible to minimize the redraws) 6 - insert ordinary pocket operations in the circles of the 'b' and the 'o' you may want to insert a 'make a group of the outlines' as step 3A (easy to select them now), then later select all the zigzags and group them, then change the group cut order to cut the zigzags first. This will give you a better edge to the letters. see attached file...
Great. Thanks to your wonderful advice, i got the issue sorted. One last thing, how would you go about getting workable files out of this design generated in illustrator and to be imported into SketchUp. The end result often ends up in a lot of unwanted paths being generated and a headache to use with SketchUCam.
Assuming you want the black in that image to stand up and everything else to be cut away, this is where a carving application shines. F-Engrave gives you this as do the various vectric apps. Also, it supports multiple bits. In this case, a 60 Vbit for crisp relief and an end-mill (straight bit) for cleaning out the bulk. Here's what I got when I brought your drawing into F-Engrave (as a PNG but no loss on detail). It's kind of hard to see what is being left but it is the the black outlined in white.
you will need to export the drawing as a DXF and import that or import the jpg and freehand draw over it in Sketchup.
in your embossed A drawing please make note of the difference between inside (blue lines), outside (orange lines) and pocket (pink lines). inside and outside cuts are intended to cut all the way through the material and use the 'overcut %' depth setting in the parameters dialog. This is a percentage of material thickness and is usually over 100% to ensure a through cut. Each pocket cut has its own depth setting in percent of material thickness. for an embossing cut like this I would avoid using inside and outside cuts entirely, and only use pocket cuts of 100% depth. Then you can change the depth of cut by changing only the 'material thickness' rather than having to remove and replace pocket cuts.
There is a thread on another site about cutting embossing dies with a cnc machine. You might want to take a look at it.
