VCarve 8.5 engraving toolpath

This forum is for general discussion regarding VCarve Pro
Post Reply
btbcobb
Posts: 4
Joined: Sun Mar 08, 2015 2:24 am
Model of CNC Machine: Axiom AR6

VCarve 8.5 engraving toolpath

Post by btbcobb »

I am trying to make a very simple text engraving. I'm using an Amana 1/16" tapered ballnose bit (#46282). Start depth is 0.0 in. Flat depth is 0.15in
However, when I hover over the toolpath that has been created the maximum depth is shown as 0.0081 in. When I run it on the machine the bit barely scratches the surface of the practice piece. I'm using 4/4 maple if it matters.

User avatar
Rcnewcomb
Vectric Archimage
Posts: 5886
Joined: Fri Nov 04, 2005 5:54 am
Model of CNC Machine: 24x36 GCnC/WinCNC with ATC
Location: San Jose, California, USA
Contact:

Re: VCarve 8.5 engraving toolpath

Post by Rcnewcomb »

Are you selecting the Quick Engraving Toolpath, or the V-carve toolpath, or some other toolpath?

If you can post the CRV file that would be best.
- Randall Newcomb
10 fingers in, 10 fingers out, another good day in the shop

User avatar
adze_cnc
Vectric Wizard
Posts: 4324
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: VCarve 8.5 engraving toolpath

Post by adze_cnc »

btbcobb wrote:I'm using 4/4 maple if it matters.
I think it matters more that you're trying to do a text engraving with a ball-end (albeit tapered) bit. Getting any depth and definition to the cuts will be difficult depending on the size of the text.

User avatar
sharkcutup
Vectric Wizard
Posts: 2885
Joined: Sat Mar 26, 2016 3:48 pm
Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
Location: U.S.A.

Re: VCarve 8.5 engraving toolpath

Post by sharkcutup »

Without a copy of your posted file here on this forum we all are just guessing at the various possibilities of your problem!

Please post/upload your .crv file here to the forum.

Sharkcutup
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 11.554

btbcobb
Posts: 4
Joined: Sun Mar 08, 2015 2:24 am
Model of CNC Machine: Axiom AR6

Re: VCarve 8.5 engraving toolpath

Post by btbcobb »

Thank You all for your replies

I think I have discovered the problem. I didn't know that entering a value for the Flat Depth defaulted to a certain depth.
I zeroed the Flat Depth then entered a non zero value in Start Depth. I then changed the tool cutting parameters to half of the Start depth.
This seems to have solved my problem.
Joe Megan 05 yahei.crv
(725 KiB) Downloaded 107 times
ADZ What tool would you recommend?

Thanks again for your help!

User avatar
Adrian
Vectric Archimage
Posts: 14541
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: VCarve 8.5 engraving toolpath

Post by Adrian »

You should have the start depth as zero. The actual cut depth on a Vcarve/engraving toolpath is set by the combination of the distance between the vectors (the individual letters) and the angle of the bit. Making the letters bigger will cut deeper as will using a more acute angle bit. The flat depth only comes into play if it's less than the actual cut depth that would be reached without it.

Because you've told the toolpath to start below the surface of the material you are now getting more cut depth. With a small ball nose you'll get away with that but with a v-bit you would end up with the letters merging into each other.

For text that small I would use a profile toolpath with single line text rather than a VCarve/engraving toolpath.

User avatar
adze_cnc
Vectric Wizard
Posts: 4324
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: VCarve 8.5 engraving toolpath

Post by adze_cnc »

btbcobb wrote:ADZe What tool would you recommend?
First: you mentioned in the original post that you were using an Amana #46282 tapered ball-end bit. Your toolpaths, though, are trying to use a 1/16" straight ball-end bit. It doesn't help much, though, to change to a real 5.4 degree 1/16 dia tapered ball-end bit.

Second: if you're going to do a "v-carve/engraving" toolpath how about using a v-bit? Duplicate your "VCarve 4" toolpath. Get rid of the start depth of 0.05", deselect flat depth check box, and for the tool select, say, a 60 deg v-bit and see how you like the result. (Looked great when I tried it).

Third: to double-check---the "Joe Megan05" is using a different typeface (more script-like) than "VCarve 4" (sans serif and very upright). Which one were you thinking of using? The v-bit with the script typeface would also look nice.

Steven

btbcobb
Posts: 4
Joined: Sun Mar 08, 2015 2:24 am
Model of CNC Machine: Axiom AR6

Re: VCarve 8.5 engraving toolpath

Post by btbcobb »

Steven,
Thanks for the suggestions and insight into the process. I find the the tutorials to be helpful to a degree. What I really find annoying is the messages I get when something is not set correctly. I understand every word in the sentence but have no context do understand what is wrong. I tried the v-bit as you suggested. I like it as well. I will try it out tomorrow. I am leaning towards the script font as well.

Thanks again for you assistance.

Brad

btbcobb
Posts: 4
Joined: Sun Mar 08, 2015 2:24 am
Model of CNC Machine: Axiom AR6

Re: VCarve 8.5 engraving toolpath

Post by btbcobb »

Adrian,

Thanks for the suggestions. I agree that the profile tool pass is simpler to work with.
Thanks for your explanation of how different factors contribute to how depth of cut is determined by the software.
It was a mystery to me.

Thanks, Brad

Post Reply