V-Carve Inlay Tear Out
-
- Vectric Apprentice
- Posts: 73
- Joined: Tue Nov 05, 2019 2:31 am
- Model of CNC Machine: Axiom Basic
V-Carve Inlay Tear Out
.13 Start Depth
.08 Flat Depth
My first one was .15 start and .1 flat. 10IPM plunge and 30IPM feed at 18,000 RPM.
- Rcnewcomb
- Vectric Archimage
- Posts: 5928
- Joined: Fri Nov 04, 2005 5:54 am
- Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
- Location: San Jose, California, USA
- Contact:
Re: V-Carve Inlay Tear Out
Using sanding sealer, shellac, etc. before cutting can help.
Maple should work better than pine.
I'd also slow down the RPMs since you are moving fairly slowly -- perhaps 12K RPM
Maple should work better than pine.
I'd also slow down the RPMs since you are moving fairly slowly -- perhaps 12K RPM
- 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
- martin54
- Vectric Archimage
- Posts: 7355
- Joined: Fri Nov 09, 2012 2:12 pm
- Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
- Location: Kirkcaldy, Scotland
Re: V-Carve Inlay Tear Out
Your running pretty slow so as Randall has suggested slow the RPM a bit, sanding sealer can help but you might need to apply it a couple of times with a 0.2 total depth. What DOC are you using for this? You could try reducing it to see if that helps, I try to keep the DOC fairly shallow if I am cutting thin lettering or graphics
-
- Vectric Apprentice
- Posts: 73
- Joined: Tue Nov 05, 2019 2:31 am
- Model of CNC Machine: Axiom Basic
Re: V-Carve Inlay Tear Out
.1 DOC, but the start depth I tried .15, .14 and .13. I just put a few coats of shellac on a test board. I will play around with it tomorrow. Thanks
-
- Posts: 20
- Joined: Thu Mar 04, 2021 1:24 pm
- Model of CNC Machine: IS 510 Shope Sabre
Re: V-Carve Inlay Tear Out
How many flutes does your end-mill have?
Your RPM is far too high and your feed rate is far too low. At the current settings you're basically burnishing the wood you're cutting and hence destroys the life of your cutter. A 1/8" 2 flute end-mill (flat nose) can easily be cutting around 100-250 IPM depending on the material you're cutting (solid wood vs plywood) at 16-18000 RPM. The feed rate will drop drastically if the wood is much harder (oak, bamboo, etc).
The Feed to RPM ratio will help with your cuts but at the end of the day your tear out is nearly inevitable. The tear out is due to the way the grain of the wood is relative to your cuts. The alternative (besides attempting to seal it followed by cutting) is to change the orientation of the board relative to your design.
Another thing that might help is "scoring" the inside edge before milling it to help avoid the tear out. Besides that, it also depends what order you're milling. Sometimes cutting out the contour edge first might be better, sometimes pocketing then milling the edge is better. From what you're doing it seems that the 22 degree edge should be milled first, then pocketing out the inside with a flat nose.
Your depth of cut seems fine.
I hope this helps.
Your RPM is far too high and your feed rate is far too low. At the current settings you're basically burnishing the wood you're cutting and hence destroys the life of your cutter. A 1/8" 2 flute end-mill (flat nose) can easily be cutting around 100-250 IPM depending on the material you're cutting (solid wood vs plywood) at 16-18000 RPM. The feed rate will drop drastically if the wood is much harder (oak, bamboo, etc).
The Feed to RPM ratio will help with your cuts but at the end of the day your tear out is nearly inevitable. The tear out is due to the way the grain of the wood is relative to your cuts. The alternative (besides attempting to seal it followed by cutting) is to change the orientation of the board relative to your design.
Another thing that might help is "scoring" the inside edge before milling it to help avoid the tear out. Besides that, it also depends what order you're milling. Sometimes cutting out the contour edge first might be better, sometimes pocketing then milling the edge is better. From what you're doing it seems that the 22 degree edge should be milled first, then pocketing out the inside with a flat nose.
Your depth of cut seems fine.
I hope this helps.
-
- Posts: 20
- Joined: Thu Mar 04, 2021 1:24 pm
- Model of CNC Machine: IS 510 Shope Sabre
Re: V-Carve Inlay Tear Out
I wanted to add that you can use the following calculators to give you a starting point as to how fast to run your cutters/end-mills.
Calculator
https://www.precisebits.com/calc
Calculator and Chip load chart
https://cutter-shop.com/
Other calculators:
https://www.kennametal.com/us/en/resour ... -feed.html
Calculator
https://www.precisebits.com/calc
Calculator and Chip load chart
https://cutter-shop.com/
Other calculators:
https://www.kennametal.com/us/en/resour ... -feed.html
- Adrian
- Vectric Archimage
- Posts: 14683
- Joined: Thu Nov 23, 2006 2:19 pm
- Model of CNC Machine: ShopBot PRS Alpha 96x48
- Location: Surrey, UK
Re: V-Carve Inlay Tear Out
The tool database will do the chip load calculations for you if you know the chipload range from the manufacturers tables.
- adze_cnc
- Vectric Wizard
- Posts: 4380
- Joined: Sat Jul 27, 2013 10:08 pm
- Model of CNC Machine: AXYZ 4008
- Location: Vancouver, BC, Canada
Re: V-Carve Inlay Tear Out
I'm curious. Is this image of the "pocket side" (a.k.a. female)? It does look like it is cut so that a plug (a.k.a. male) piece would fit into it.
If it is indeed the pocket that the inlayed plug will be glued into the question I have would be:
Why start depth 0.13 and flat depth 0.08? With the plug (female) side you can use start depth 0 and flat depth 0.21. That way, if your v-bit has a stepdown of less than 0.21 it won't try to cut to full depth in one go.
-
- Posts: 20
- Joined: Thu Mar 04, 2021 1:24 pm
- Model of CNC Machine: IS 510 Shope Sabre
Re: V-Carve Inlay Tear Out
Not to beat the same drum on the chip load/feed rate/RPM issue but keep in mind that this is just a starting place.
For example, I have two 3 flute compression endmills, one from Whiteside (looks bulkier) and one from an unknown manufacturer (which is quite good). The Whiteside endmill is programmed at 10700 RPM at 450 IPM and the unknown manufacturer one is at 13250 RPM at 450 IPM. The Whiteside endmill has a lower cutting maximum than the unknown manufacturer endmill (which I've easily run at 18000 RPM at 2000 IPM).
So it all depends on how the sharpening was done, the kinds of angles they made, etc on the mill itself. Not to mention the material its made of. So the chipload can vary greatly (whiteside: 0.014 vs Unknown: 0.0113). Also the higher the chip load can be without breaking the tool (if you're satisfied with the finish) the longer the tool will last because it can dissipate heat better.
For example, I have two 3 flute compression endmills, one from Whiteside (looks bulkier) and one from an unknown manufacturer (which is quite good). The Whiteside endmill is programmed at 10700 RPM at 450 IPM and the unknown manufacturer one is at 13250 RPM at 450 IPM. The Whiteside endmill has a lower cutting maximum than the unknown manufacturer endmill (which I've easily run at 18000 RPM at 2000 IPM).
So it all depends on how the sharpening was done, the kinds of angles they made, etc on the mill itself. Not to mention the material its made of. So the chipload can vary greatly (whiteside: 0.014 vs Unknown: 0.0113). Also the higher the chip load can be without breaking the tool (if you're satisfied with the finish) the longer the tool will last because it can dissipate heat better.
- rink
- Vectric Craftsman
- Posts: 188
- Joined: Tue Jul 07, 2020 3:45 pm
- Model of CNC Machine: OpenBuilds LEAD 1510 / VCarve Pro
- Location: USA
- Contact:
Re: V-Carve Inlay Tear Out
Good evening everyone.
I’m not the expert on this forum, as Randall, Martin, Adrian and others are. But here’s a thought.
I routinely run about that same feed/speed/plunge with a 1/8 inch shaft, 30 degree v-bit, on solid walnut, cherry, and white oak for inlay and other work. It works fine on my very small Nextwave CNC Piranha. Although, I have had a few chipouts, especially where the grain lines and a change in router direction didn’t agree.
But when doing V-Carve (or Zank) inlays there’s another consideration for the MALE inlay piece, and that’s your start depth. There’s been a lot written about it on this forum, in fact there’s a 20-something page thread on it that is very educational.
Anyway, the point is that I think your start depth and your z-zero may be contributing to your problem. In addition to your tool-specific pass depth, the machine will cut that depth PLUS your start depth on the first pass. That may be too much.
My method for this type of inlay is to zero my bit at 0.08” above the workpiece, then run the job. Then I lower the bit 0.04” and run the job again. Then lower another 0.4” and make the final run. This is for a female pocket of 0.1” and a male inlay of start depth 0.08” and flat depth of about 0.1” or so. It’s time-consuming and tedious to make three runs, and there’s a lot of cutting air on passes #2 and #3, but the quality is good and I’m not on anyone’s schedule or deadline by my own
You may already know all of this, as I said I’m not the expert and still early in my learning curve. The other guys should feel free to correct me here, but it is something you should probably add to your consideration.
Thx, rink.
I’m not the expert on this forum, as Randall, Martin, Adrian and others are. But here’s a thought.
I routinely run about that same feed/speed/plunge with a 1/8 inch shaft, 30 degree v-bit, on solid walnut, cherry, and white oak for inlay and other work. It works fine on my very small Nextwave CNC Piranha. Although, I have had a few chipouts, especially where the grain lines and a change in router direction didn’t agree.
But when doing V-Carve (or Zank) inlays there’s another consideration for the MALE inlay piece, and that’s your start depth. There’s been a lot written about it on this forum, in fact there’s a 20-something page thread on it that is very educational.
Anyway, the point is that I think your start depth and your z-zero may be contributing to your problem. In addition to your tool-specific pass depth, the machine will cut that depth PLUS your start depth on the first pass. That may be too much.
My method for this type of inlay is to zero my bit at 0.08” above the workpiece, then run the job. Then I lower the bit 0.04” and run the job again. Then lower another 0.4” and make the final run. This is for a female pocket of 0.1” and a male inlay of start depth 0.08” and flat depth of about 0.1” or so. It’s time-consuming and tedious to make three runs, and there’s a lot of cutting air on passes #2 and #3, but the quality is good and I’m not on anyone’s schedule or deadline by my own
You may already know all of this, as I said I’m not the expert and still early in my learning curve. The other guys should feel free to correct me here, but it is something you should probably add to your consideration.
Thx, rink.
I want to be unique like everyone else.
-
- Vectric Craftsman
- Posts: 130
- Joined: Tue Feb 06, 2018 9:18 pm
- Model of CNC Machine: CNC 6040, Vectric Aspire, UCCNC
- Location: Skane, Sweden
Re: V-Carve Inlay Tear Out
Would it not be simpler to create three toolpaths with three different start depth and combine them into one when saving?
- rink
- Vectric Craftsman
- Posts: 188
- Joined: Tue Jul 07, 2020 3:45 pm
- Model of CNC Machine: OpenBuilds LEAD 1510 / VCarve Pro
- Location: USA
- Contact:
Re: V-Carve Inlay Tear Out
Well, duh.mickecarlsson wrote: ↑Thu Sep 23, 2021 9:37 amWould it not be simpler to create three toolpaths with three different start depth and combine them into one when saving?
Yes, I suppose that would be simpler at run time and immaterially more work at toolpath creation time. I hadn’t thought about it that far. I guess the run time would still be long but I wouldn’t have to manually reset the Z-zero each time.
Thanks for the tip. What a great forum!
Thx, rink.
I want to be unique like everyone else.
- martin54
- Vectric Archimage
- Posts: 7355
- Joined: Fri Nov 09, 2012 2:12 pm
- Model of CNC Machine: Gerber 48, Triac PC, Isel fixed gantry
- Location: Kirkcaldy, Scotland
Re: V-Carve Inlay Tear Out
I don't do a lot of inlays & haven't done one for some time now but in another post Adrian said there was now a gadget to help with this, not actually read it but this is the post Adrian linked to when he mentioned the gadgetrink wrote: ↑Thu Sep 23, 2021 1:52 pmWell, duh.mickecarlsson wrote: ↑Thu Sep 23, 2021 9:37 amWould it not be simpler to create three toolpaths with three different start depth and combine them into one when saving?
Yes, I suppose that would be simpler at run time and immaterially more work at toolpath creation time. I hadn’t thought about it that far. I guess the run time would still be long but I wouldn’t have to manually reset the Z-zero each time.
Thanks for the tip. What a great forum!
Thx, rink.
viewtopic.php?f=51&t=38177