I am running Vcarve Desktop V9.510 and I am using Mach 3 with an A rotary axis. My question is how can I reduce wasted cutting time? I model a 3D part, something like a hatchet handle, in Onshape, and then import it in and 3D rough and finish cut it on my rotary axis. It works just fine. The question I have is how could I start with a rectangular piece of stock instead of a round one? My part is basically an ellipse. When it goes to rough out the ellipse shape out of a round, and I am using a rectangular stock piece(real part on the CNC), I cut a lot of air where the rectangle is smaller than the starting round shape in software. I would like to either be able to specify a rectangular stock part or take the specified round part and make a first cut to make it rectangular and then from the rectangular shape I would do my rough and finish cuts to make the part I want. I would then just ignore the first cut, to make the round stock rectangular and then do my actual rough and finish cuts.
I am open to any other ideas or if my second idea would work can you help me with how I would fake it out to make a rectangular part from a round and then continue on with my shape. I don't know how to sketch a rectangle on the end of the part to make the part a rectangle but in a 2D view of the unwrapped rotary part.
I am assuming that Vectric is not looking to change the initial stock shape for a rotary job but I can hope.
Thanks for any help you can provide.
Scott
Rectangular stock for a rotary job
- Rcnewcomb
- Vectric Archimage
- Posts: 5887
- Joined: Fri Nov 04, 2005 5:54 am
- Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
- Location: San Jose, California, USA
- Contact:
Re: Rectangular stock for a rotary job
Skip the roughing. If you need to reduce material to avoid breaking a bit then don one finish pass with a large diameter bit and a larger stepover. Finish passes are always at full depth. Roughing passing will always attempt to remove stock it believes is there,
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop
10 fingers in, 10 fingers out, another good day in the shop
- SRiddle68
- Posts: 10
- Joined: Sun Nov 18, 2018 9:37 pm
- Model of CNC Machine: Homemade CNC w/Mach4
- Location: Pella, IA 50219
Re: Rectangular stock for a rotary job
My spindle is not super rigid and I have it pretty much maxed out feed rate and depth wise now, so how I do the cutting doesn't matter. But regardless of the strategy I use to cut it, it wastes a ton of time cutting air.
See the attached picture for a better understanding of what I mean. 2/3 of the time to cut this part will be just cutting air, not wood.
Thanks
Scott
See the attached picture for a better understanding of what I mean. 2/3 of the time to cut this part will be just cutting air, not wood.
Thanks
Scott
- Rcnewcomb
- Vectric Archimage
- Posts: 5887
- Joined: Fri Nov 04, 2005 5:54 am
- Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
- Location: San Jose, California, USA
- Contact:
Re: Rectangular stock for a rotary job
It will not air cut if you just use finishing passes. You can run more than one finishing pass if needed.
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop
10 fingers in, 10 fingers out, another good day in the shop
- SRiddle68
- Posts: 10
- Joined: Sun Nov 18, 2018 9:37 pm
- Model of CNC Machine: Homemade CNC w/Mach4
- Location: Pella, IA 50219
Re: Rectangular stock for a rotary job
The problem is that I cant go full depth to the final part size. In the attached picture, the final part is in green. You can see the corners would be almost a .50" deep cut if it went full depth. I can only do about a .125 deep cut with a 50% step over on a .25 dia ball nose carbide router bit.
I appreciate your help on this. It helps me a ton to get other thoughts and ideas.
Scott
I appreciate your help on this. It helps me a ton to get other thoughts and ideas.
Scott
- mtylerfl
- Vectric Archimage
- Posts: 5865
- Joined: Thu Jan 29, 2009 3:54 am
- Model of CNC Machine: -CarveWright CNC -ShopBot Buddy PRSAlpha
- Location: Brunswick, GA
Re: Rectangular stock for a rotary job
Perhaps this job is better suited for two-sided machining?
Michael Tyler
facebook.com/carvebuddy
-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
facebook.com/carvebuddy
-CarveWright CNC
-ShopBot Buddy PRSAlpha CNC
- rscrawford
- Vectric Wizard
- Posts: 1102
- Joined: Mon Jan 17, 2011 6:49 pm
- Model of CNC Machine: CAMaster Cobra 408 ATC, ShopSabre IS408
- Location: Wetaskiwin, Alberta
- Contact:
Re: Rectangular stock for a rotary job
Why can't you cut more than 1/2" depth for your finish tool path?
I just finished a 3D cut, and I was making 2.5" deep cuts with a 1/2" ball nose. It is really not much of a cut, because I was only taking off 7% per pass, or 0.035" per cut.
With a 1/4" ball nose, you should easily cut 3/4" depth as long as you keep your stepover under 10%. Use a raster, so you start at one end and work your way up the 4th axis.
I just finished a 3D cut, and I was making 2.5" deep cuts with a 1/2" ball nose. It is really not much of a cut, because I was only taking off 7% per pass, or 0.035" per cut.
With a 1/4" ball nose, you should easily cut 3/4" depth as long as you keep your stepover under 10%. Use a raster, so you start at one end and work your way up the 4th axis.
Russell Crawford
http://www.cherryleaf-rustle.com
http://www.cherryleaf-rustle.com
-
- Vectric Wizard
- Posts: 1701
- Joined: Sun Sep 23, 2012 12:14 pm
- Model of CNC Machine: CNC Shark Pro, Probotix Meteor 25" x 50"
Re: Rectangular stock for a rotary job
I'm with Michael. This looks like a great excuse for 2-sided carving. I'd start with a block 7/4 thick, a couple inches longer than you need the finished part. Clamp or screw down the ends parallel to one axis of your CNC. The moulding toolpath could be used to cut the top side. Flip the blank over end for end, screw down again and use the same toolpath for the bottom side (now on top).
4D
4D
- SRiddle68
- Posts: 10
- Joined: Sun Nov 18, 2018 9:37 pm
- Model of CNC Machine: Homemade CNC w/Mach4
- Location: Pella, IA 50219
Re: Rectangular stock for a rotary job
Russell's idea would work if my CNC had the rigidity for that heavy of a cut. I can only do about a 1/8 deep with 50% stepover and 40 FPM. If I go more it chatters like crazy and I end up losing steps on the motor. This is a light machine, not a large industrial one. I am working on a lathe that will be able to take very heavy cuts with live tooling but that is months off.
I like the 2 sided idea and just use X,Y,Z moves than flip and repeat. The next wrinkle I have is I project a cross-hatch pattern of lines on the surface of the ellipse. I then use a 60 deg v-carve bit to trace the lines. The bit is always perpendicular to the surface when rotating the part. If I do a 2 sided operation and go to v-carve the cross hatch lines projected onto the ellipse the bit would not be perpendicular to the curved surface always. I probably could make it as 2 separate Vcarve projects. The first would be 2 sided in flat mode and then just do the cross-hatching v-carve work as a rotary project.
I like the 2 sided idea and just use X,Y,Z moves than flip and repeat. The next wrinkle I have is I project a cross-hatch pattern of lines on the surface of the ellipse. I then use a 60 deg v-carve bit to trace the lines. The bit is always perpendicular to the surface when rotating the part. If I do a 2 sided operation and go to v-carve the cross hatch lines projected onto the ellipse the bit would not be perpendicular to the curved surface always. I probably could make it as 2 separate Vcarve projects. The first would be 2 sided in flat mode and then just do the cross-hatching v-carve work as a rotary project.
- martin54
- Vectric Archimage
- Posts: 7339
- Joined: Fri Nov 09, 2012 2:12 pm
- Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
- Location: Kirkcaldy, Scotland
Re: Rectangular stock for a rotary job
Have you tried reducing the stepover? Russell said to take a deeper cut but at a smaller stepover
Worth spending a bit of time experimenting with the software to see how it affects carving time
Worth spending a bit of time experimenting with the software to see how it affects carving time