[noisillator]

Can Cut2D create a hole like this, importing a DXF from AutoCAD 2000? It's about 2" diameter. Note the fillet around the top edge. Also, the actual hole might be D-shaped, rather than round.

[lovebugjunkie]

I use VcarvePro and it cannot do the fillet as a tool path that I know of, so I'm pretty sure Cut2D will not be able to. Might want to ask on the Vcarve forum to verify.

[noisillator]

I use VcarvePro and it cannot do the fillet as a tool path that I know of, so I'm pretty sure Cut2D will not be able to. Might want to ask on the Vcarve forum to verify.

VcarvePro is out of my price range for the time being. Do you know of any other CAM software (inexpensive) that might have this capability?

[ger21]

There is a way to do it, but it's not easy. You need to calculate the toolpaths yourself, and draw each one as an offset line from the actual hole, in the correct offset location. Here's how I'd do it.

Draw a side view of the edge detail. That's the blue line. Now, offset the blue line up by the tool radius. That's the green line. Now, where the hole is cut through, you'll have a toolpath offset by the tool radius. Far right vertical line. Draw a series of lines with the spacing being the stepover. Trim them off below the green line. Now, as you can see, the bottom of the lines where they were trimmed, is the center of the ballnose tool. This is where the drawing stops.

Now, move all the vertical lines down by a distance equal to the tool radius. The top of your part (Blue line) is Z=0. The bottom of the vertical lines is the depth of cut of each pass.

So take a top view 2D drawing, and draw a line offset inside the hole by a distance of the tool radius. Then offset from that back towards the part by the stepover distance, as many passes as you want. Put each offset line on it's own layer and include the depth in each layer name.

In Cut 2D, create a toolpath from each vector cutting to the depth you used in the layer name.

A bit tedious, but doable. I use this frequently at work to make custom moldings and countertop edges. One benefit of this is it'll have far fewer lines of code, and cut much faster, than if you used a 3D CAM program on it

[mcphill]

VcarvePro is out of my price range for the time being. Do you know of any other CAM software (inexpensive) that might have this capability?

What do you consider "inexpensive"? You can talk BobCAD down to $600 or less.

[ger21]

VcarvePro is out of my price range for the time being. Do you know of any other CAM software (inexpensive) that might have this capability?

He said V Carve Pro can't do it.

[BobF]

1. Just cut the hole with Vectric and use a handheld with bearing guided roundover bit to do the fillet.

2. Use a 1/2" bit to cut the hole profile with CAM, and 1/2" bearing guided roundover for the fillet following the same toolpath as the profile toolpath.
No I haven't tried 2 and if your bearing and cutter are not the same diameter it won't work for sure.

[noisillator]

What do you consider "inexpensive"? You can talk BobCAD down to $600 or less.

Well, this has to be scaled a bit to fit with the system I'm assembling (Taig) and the intended use (hobby). I was hoping for something in the region of $150.

[noisillator]

He said V Carve Pro can't do it.

He said it can't do it that he knows of. Isn't that the reason he suggested I check the Vcarve forum, to clarify that point? Thanks for posting the manual technique for getting this done. I need to mull that over to be sure I understand everything involved.

[noisillator]

1. Just cut the hole with Vectric and use a handheld with bearing guided roundover bit to do the fillet.

I do have woodworking routers and a table, but I worry about the quality of the work with this method. There are several potential issues, probably too OT for this forum (and likely discussed in-depth by others elsewhere). I will keep this one in the back of my mind though as a last resort sort of thing.

2. Use a 1/2" bit to cut the hole profile with CAM, and 1/2" bearing guided roundover for the fillet following the same toolpath as the profile toolpath.
No I haven't tried 2 and if your bearing and cutter are not the same diameter it won't work for sure.

Do you mean to use the CNC and change tools? I wouldn't want to use a bearing in that case, would I? This might be a pretty good alternative, especially as I'm not planning to cut a lot of holes like that.

This reminds me, is there any problem cutting a blind hole with an end mill using Cut2D? Can I mix through-holes and blind holes on the same panel in the same pass (same tool)?

[blowlamp]

Hi.
I'm 99% sure that CamBam can do this. Take a look at the example screenshot of the toolpath I generated in CamBam. Simple to do too.

Cheers.
Martin.

[LeeWay]

They do sell round over end mills too. That might get you there cheaper than the software especially for one off's. I generally campher using a mill drill. I use Sheetcam for this. The same type code should work for a round over. May take a few shallow test passes at first, but could could be zeroed in pretty well.

[noisillator]

Hi.
I'm 99% sure that CamBam can do this. Take a look at the example screenshot of the toolpath I generated in CamBam. Simple to do too.

Cheers.
Martin.

Martin, did you import that into CamBam or create it within the program? I wasn't able to do any 3D work in CamBam, although I admit to not spending a lot of time with it.

[blowlamp]

It was all created within CamBam, but could easily have started with a cad drawing.
I drew a circle and while still highlighted, applied a Profile machining operation to it. I changed the SideProfile property to ConvexRadius and set the Value parameter to something sensible that could be used in that particular size of circle. I also set the DepthIncrement (keep this value small for good resolution), TargetDepth (put a minus sign in front of this number), and ToolDiameter to something usable too. Right click in the drawing window and select Machining > Generate Toolpaths and if you've entered good values for ToolDiameter etc, you should get something to work with. This can be applied to just about any shape, not just circles, so should do what you're after.

Cheers.
Martin.

[High Seas]

1. Generate the CAD drawing
2. Save as an STL File
3. Launch STLWORK
4. Pick tool ( as I recall you can make it a round-over bit too)
5. Generate the G-Code choice of X-Y, Y-X, or waterline (it also slabs)
6. Trial run on a back-plotter (NCPLOT/CAMBAM etc)
7. Cut the piece
8. Admire your handiwork

Thats how I'd approach it - Just my 2C and STLWORK is less than a hundred bucks -- but many of you have heard before- not associated -- it just works for me!.
Cheers - Jim

BTW -- I think you can still get a demo file downloaded. (http://www.cadcamcadcam.com/othersoftware.aspx) oops its now $125....