v carve and pocket toolpaths not cutting to lines

This forum is for general discussion about Aspire
Post Reply
markost
Posts: 3
Joined: Mon Sep 13, 2021 11:30 am
Model of CNC Machine: diy centroid acorn

v carve and pocket toolpaths not cutting to lines

Post by markost »

Hi
I have tried v carving a chechered emblem and also with pocket toolpath same problem occurs, i used a friends ver 9.5 with a 20deg engraving bit with succes cutting to lines but when i purchased ver-11 it will not let me cut to the line it cuts short as i need cut every alternate square and come back the following day and cut the opposite squares. thanks in advance
regards marko
left v-9.5 ,right ver-11
left v-9.5 ,right ver-11
IMG_3305.jpg
new grb dxf 9.5.crv3d
(568.5 KiB) Downloaded 32 times

User avatar
Adrian
Vectric Archimage
Posts: 14547
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: v carve and pocket toolpaths not cutting to lines

Post by Adrian »

Have you got the bit correctly defined? You say it's a 20 degree bit but is that the total angle or the side angle? With an engraving bit you enter the side angle and with a v-bit you enter the total angle.

The previews (both 3D and solid 2D) are correct so you're either using a different bit from what VCarve has been told or there is another issue with your machine or process.

markost
Posts: 3
Joined: Mon Sep 13, 2021 11:30 am
Model of CNC Machine: diy centroid acorn

Re: v carve and pocket toolpaths not cutting to lines

Post by markost »

Hi thanks for that will change all engraving bits to v carve definition

User avatar
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: v carve and pocket toolpaths not cutting to lines

Post by martin54 »

markost wrote:
Tue Sep 14, 2021 9:15 am
Hi thanks for that will change all engraving bits to v carve definition
If I understand what you have said correctly then entering your engraving bits as V bits is not a good idea (generally) because the software assumes a V bit comes to a point & doesn't take the flat into account which may give you strange results. What you need to do is make sure you have them set up correctly in the tool database.
As Adrian has pointed out V bits are entered using the included angle of the bit & engraving bits entered using the side angle of the bit (half the included angle) :lol: :lol: :lol:

markost
Posts: 3
Joined: Mon Sep 13, 2021 11:30 am
Model of CNC Machine: diy centroid acorn

Re: v carve and pocket toolpaths not cutting to lines

Post by markost »

Make perfect sense
Thanks

User avatar
scottp55
Vectric Wizard
Posts: 4713
Joined: Thu May 09, 2013 11:30 am
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP11.5
Location: Kennebunkport, Maine, US

Re: v carve and pocket toolpaths not cutting to lines

Post by scottp55 »

Yep, to start enter bits exactly as they are for an accurate preview!
For instance, a VBit stepover is a percentage of tool Diameter.
An Engraving bit stepover is a percentage of the Tip Flat!
It can Muck up a cut in short order.

I Do have most of my small tip flats Engraving bits entered as VBits ALSO for exceptions,
BUT you have to have a picture in your head that it will cut deeper and shave the sides a hair.
Best to stick with an accurate tool description, so an accurate preview saves you a workpiece!
(Don't ask how I know!) :)
scott
I've learned my lesson well. You can't please everyone,so you have to please yourself
R.N.

User avatar
adze_cnc
Vectric Wizard
Posts: 4329
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: v carve and pocket toolpaths not cutting to lines

Post by adze_cnc »

scottp55 wrote:
Sun Sep 19, 2021 8:02 am
For instance, a VBit stepover is a percentage of tool Diameter.
An Engraving bit stepover is a percentage of the Tip Flat!
That's why I rarely think about step-overs in terms of percentages. I pretty much always think in terms of absolute distances (e.g. 0.03 inches) that way it doesn't really matter how the Vectric programs derive the percentage. An exception is hogging out large areas with large cutters.

It's fun seeing people say "I set the step-over to 1%" and you realize that it's 1/10.000 inch and you know that their machine's stepper motors only have a resolution of 1/1,000 inch so they're doing 9 passes with little effect.

Post Reply