LinkBack URL
About LinkBacks
Anyone?
I've tried the SprutCAM user forum as well but have been having trouble accessing it lately.
Mike
| | |
I'm attempting to do an engraving project and would like to make 2 passes on the line art, one with conventional milling and the other with climb milling. The engraving spindle is non-reversible so I'd like to make a pass between endpoints of a line segment and then back again to the starting endpoint.
The "Machining with Return" feature works fine for this on straight line segments. On open curved lines (like arcs or polylines), the Return feature doesn't reverse the cutter path, but loops around to the origin once it reaches the endpoint. An arc in the form of a half circle gets milled as a full circle.
I'm using a 2D Contouring operation for the line art. Is there a way to make both conventional and climb passes with this operation on arcs, should I be using a different type of operation, or am I out of luck.
Mike
Anyone?
I've tried the SprutCAM user forum as well but have been having trouble accessing it lately.
Mike
Hi Mike, I suspect that you are using the wrong function.
De-select the 'Return' option that you are selecting (curve).
To achieve what I think you are trying to do, in the Strategy window of the 2D contouring operation, enable the 'Reverse direction' option and set the 'Transition' option to 'Around workpiece'.
I'm not sure why you would want to reverse the spindle?
Dave
Hi Dave,
Guess I could have explained that better. The project has some line art that consists in part of open lines, spirals, and arcs. I'm using an engraving bit (1/8" dia, 60°, 0.005" tip) to engrave the line art on acrylic sheet 0.005" deep with a spindle that is non-reversible. The engraved line art has a burr on one side of the mill path and I'd like to make 2 passes per line, spiral, or arc segment so that each side of the line, etc gets both conventional and climb passes in an attempt to eliminate or at least minimize those burrs.
The "Machine with Return" works perfectly on the straight line segments but on an open arc, it creates a closed arc on the "Return" segment. For example, if the art includes a half circle, "Machine with Return" mills a complete circle whereas I'd like it to mill the half circle twice, starting at the arc origin, proceeding to the arc endpoint and then back to the arc origin along the same path.
I've tried deselecting the Return, enabled Reverse direction, and set the transition to around workpiece, but that apparently mills the blank space between the individual line, spiral, or arc segments. I'll play around with it some more to see if there's something else I can do.
In the meantime here is an example of the project which will hopefully give you a better idea of the issue:
Mike, I don't use it much myself, but have you tried the engraving operation?
I think that if you assign your curves as 'Ditch' it should do what you need for open or closed curves.
I have put a screengrab taken from SprutCAM 2007 here
Dave,
Thanks - that seems to work pretty well, at least so far as simulation goes. I'm not sure why but selecting "Ditch" for the engraving operation results in no machining at all, but using "Inversion Curve" creates two paths along a selected open curve, from curve start to end and back to start. Each path appears to slightly offset from the curve itself, but that should be fine for this project.
Mike
Mike,
Make sure that you set the tool as engraver, with the correct angle etc.
Set the side angle to the same value and set the bottom level to more than you need.
Now select the curves (ditch) that you are machining and add stock (width) to them, this will govern the depth.
Now select 'Allow 3D toolpath' (Strategy) and see if this works ok.
I found that I also had to adjust the Deviation outer figure a little to give a clean cutter path on an arc.
Dave
Thanks, that's much better. The toolpath is now right on the centerline of the line art, which should make for sharper line art, and it still makes the two passes I was looking for, which should clean up that burr.
I'm really curious how you came up with the solution, especially the part about setting bottom level deeper than needed and then adding stock back to it. That wasn't at all intuitive to me and I'm wondering if that is a standard CNC technique or something peculiar to SprutCAM. In either case it means more to learn; I'd just like to know if learning effort is better spent on CNC books or the SprutCAM manual and/or exploring the program itself.
BTW, I'm still on SC Expert 4.
Mike
Mike, I guess I've just got too much time on my hands
To understand how to use the 'Ditch' and 'Ridge' options I would suggest that you try using them in a Pocketing operation.
Just create a 2D geometry line and use this as your 'Part', set the curve as a 'Ditch' and add stock to the curve. In this example I have added 5mm stock, so the slot is 10mm wide:
If you now change it to a ridge instead you will get the inverse (male) form:
If you now add some side angle, you can see that the bottom 'self intersects' and this is what governs the depth:
CNC books are good if you want to learn the 'Black art' of G-code programming.......I prefer to just get on with it and make parts using SprutCAM
If I had more time I would write an e-book about SprutCAM........
Dave,
That provides a glimmer of understanding and I'll play with the concepts tonight after work.
If you keep answering my questions you'll be half way to that eBook soon <g>.
Thanks, Mike
Posting Permissions
| | |
