Can't do multiple depths with 2D Contour and chamfer tool

[dbeetcher]

I'm trying to use 2D Contour with a V-bit (chamfer) to engrave a pattern into an acrylic pickguard. At first I tried using the Trace toolpath, but Trace seems to turn all the curves into line segments, which caused my CNC machine to 'stutter' around the curves and produce slightly jagged cuts. So I thought I would switch to 2D Contour instead (which leaves the curves as arcs instead of line segments). To produce nice clean edges, I wanted to do a couple of shallow cuts in the acrylic. But in the Passes tab of 2D Contour, there was no Multiple Depths selection. I finally figured out that when you select a chamfer-type tool (which is how I set up my V-bit tool), the Multiple Depths option is missing. Does anyone know how to either: 1) get the Multiple Depths option back, or 2) suggest how to set up my V-bit as the type of tool that will allow the Multiple Depths option to appear in the palette? Or is there another way to solve this that I'm overlooking? I suppose I could just duplicate the 2D Contour setup a few times and make the depth of cut a little deeper for each one, but that doesn't seem very 'elegant'.

Thanks, Dan

[LibertyMachine]

Couple things you can do: 1) Turn on Smoothing in the Trace toolpath. This should go quite a ways in smoothing things out. I tend to run .0004 tolerance and smoothing and have decent results. 2) Use the 2D Contour operation and define your tool as a Tapered Mill. You will need to play with the values to get it to look correct. 3) Define your tool as a "Form Tool". You will need to sketch up the profile of half the tool (the form tool creation basically creates a "revolve" of your sketch)

[LibertyMachine]

Couple edits: 1) There are carriage returns in the above post. Forums are broken beyond belief right now 2) There are actually three suggestions, not a couple 🙂

[dbeetcher]

Hi Seth, I did have smoothing turned on. But turning it on and having the tolerance and smoothing values set correctly are two different things! I saw a post that called for the tolerance value to be 2-5 times the smoothing value. But what is the right smoothing value for my job? I'm working on a pickguard that has a lot of tiny details on it, fractions of a millimeter in size! I'll try creating a new tool as you suggested, too. Thanks, Dan

[LibertyMachine]

Could you export and share your file? File > Export > Save to local folder. Return to thread and attach the .f3d file in your reply

[dbeetcher]

Hi Seth, Sorry, didn't read your comment as closely as I should have. You recommend both tolerance and smoothing to be .0004", right? I think I had mine set to .01mm (which IS ~0.0004"). So I guess I had my values about the same as yours. I've made a new tool (tapered) as you suggested, so now I'll just see if it allows me to get multiple depths in 2D Contour or not. Dan

[dbeetcher]

Hi Seth, My drawing is kind of a mess. I've been experimenting a lot and my CAM toolpaths are all over the place, with creating some with Trace and some with 2D Contour. I'd have to do a bit of cleanup before I'd post them, otherwise they wouldn't make any sense to anyone! But I could go ahead and do that if you think it would be a major aid in solving my problem. Dan

[dbeetcher · Accepted solution]

Seth, I took your advice (most of it). I used the 2D Contour toolpath, with the tolerance and smoothing parameters set to 0.01mm. For the tool, I just selected an endmill in F360, but I actually installed a V-bit in the router (I edited the 'endmill' tool to have a 0.1mm diameter - which is the tip size of the V-bit). In the Passes tab, I set the Compensation Type to "Off", so that the V-bit would cut exactly on top of the lines. Choosing an endmill-type tool allowed me to select multiple depth passes.
I found that almost all of the splines I used in my drawing were getting converted to line segments when F360 generated my toolpaths. In general, using 2D Contour should convert the splines to arcs. But when I was doing some testing to try to figure out why line segments were being created (instead of arcs), I was doing a copy/paste of the splines from one sketch to another sketch. Apparently when you copy/paste splines, the pasted splines will NOT have exactly the same behavior as the original. Because of that, the splines were getting converted to little, short line segments. After I had re-drawn (not copy/pasted) the splines in the sketch, they were converted properly to arcs in the toolpath. And finally, I made 2 changes to my Mach3 General Configuration tab: 1) I changed the "Motion Mode" from "Exact Stop" to "Constant Velocity", and 2) I changed "Look Ahead Lines" from "20" to "200".
After these changes, all of the jerky movements of the CNC servo motors were smoothed out.
Thanks for your help, Dan