Adjust depth of V cut

This forum is for requests and queries about machine tool support for Vectric Products

Adjust depth of V cut

Postby apopj » Mon Mar 18, 2019 4:45 pm

Hello all,

I am attempting to cut a pattern onto a piece of 1/4" wood using V carved letters. The problem is, the bit goes much too deep and cuts through the wood. I also use 1/8 wood with the same problem. This is the case whether I use a 60' V bit or the 90' v bit.

In Vectric Pro/Desktop/Aspire, is there a way to reduce the depth to which the cutter digs in?

Thanks for the help,

Jeff
apopj
Vectric Apprentice
 
Posts: 10
Joined: Tue Jan 22, 2019 6:27 pm
Location: New Franklin, Ohio USA
Model of CNC Machine: Shapeoko 3 XXL

Re: Adjust depth of V cut

Postby SteveNelson46 » Mon Mar 18, 2019 4:58 pm

The depth of a v-carve is determined by the space between two lines. The bit will plunge to a depth to fill the space. You can set a flat depth so the lettering or v-carve will have flat bottoms but this may or may not achieve a desired effect.

EDIT: I just noticed this post is in post processors. Your question has little or nothing to do with post processors.
Steve
User avatar
SteveNelson46
Vectric Wizard
 
Posts: 555
Joined: Wed Jan 04, 2012 2:43 pm
Location: Tucson, Az.
Model of CNC Machine: Camaster Stinger with Recoil Lathe

Re: Adjust depth of V cut

Postby Adrian » Mon Mar 18, 2019 5:07 pm

Just to add that the less acute the angle of the bit the shallower it will cut so a 60 will cut deeper than a 90 and a 90 will cut deeper than 120. Otherwise as Steve said, make the gap between the vectors wider or set a flat depth. There are some excellent diagrams in the v-carve toolpath section of the Help Contents on the Help menu which show how it works.
User avatar
Adrian
Vectric Archimage
 
Posts: 9681
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Adjust depth of V cut

Postby apopj » Tue Mar 19, 2019 2:22 am

Well, since I couldn't find an answer here, I did a little experimenting. Here's what I found.....

None of the tutorial videos from Vectric really address the problem. As was mentioned, various angles, induces hyperbol caused by the refraction of light on the rays of the moon and other such mumbo jumbo. NOTHING explained how to reduce the depth of cut, just yada yada yada.

SOOOOOO, I played with various settings and found that by using the engrave function, you can adjust the depth of cut by entering a depth/pressure number of .01 or so. If I enter a number of .01 and use a 60' V bit, I can carve a clear name on a piece of 1/16th wood. I did a test of using pressures of .01, .02, .03, .04, and .05. All of them worked pretty well, but the .01 or .02 worked best. Try it and see what you think.....

Jeff
apopj
Vectric Apprentice
 
Posts: 10
Joined: Tue Jan 22, 2019 6:27 pm
Location: New Franklin, Ohio USA
Model of CNC Machine: Shapeoko 3 XXL

Re: Adjust depth of V cut

Postby Adrian » Tue Mar 19, 2019 8:07 am

What do you mean you couldn't find the answer here? It's one of the most commonly asked questions on the forum and a quick search will find loads of information plus Steve and I both answered the question.

It's really quite simple. The v-bit "rides" on the inner and outer vectors so if you move those vectors closer together the bit "lifts" up giving a shallower depth. Move them apart and the bit "falls" further between them cutting deeper. The same thing happens with different angle bits. A 60 degree bit will "fall" further between the same vectors as a 90 degree bit. There's also the flat depth option.

Two minutes spent playing around with different sized rectangles and the VCarve preview would have shown you exactly how it works.

The engraving toolpath does work well for very small text or thin material as does a profile on the vector cut using a single line font. If you had explained what it was you were doing (cutting 1/16" thick material) and had posted in the correct section of the forum (this is nothing whatsoever to do with post processors) then I'm 100% certain you would have got answers straightaway that you might have found more satisfactory.

I notice in the other thread that you posted with more details and in the correct section Mark advised using the Quick Engrave toolpath some hours before you posted your reply above.....
User avatar
Adrian
Vectric Archimage
 
Posts: 9681
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Adjust depth of V cut

Postby Adrian » Tue Mar 19, 2019 8:59 am

Forgot to mention it's also covered in the FAQ - http://support.vectric.com/aspire-quest ... or-shallow
User avatar
Adrian
Vectric Archimage
 
Posts: 9681
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Adjust depth of V cut

Postby Rcnewcomb » Tue Mar 19, 2019 8:24 pm

In Vectric Pro/Desktop/Aspire, is there a way to reduce the depth to which the cutter digs in?

Your various options are:

Use a V bit with a wider angle. The wider the angle, the shallower the cut. Gerber, for example, makes V-bits with angles as large as 150°
VbitDepth.png


Use a ballnose bit. When you select a ballnose bit for V-carving the tool will go no deeper than the radius of the ballnose. A 1/8" diameter ballnose (1/16" radius) will carve no deeper than 0.0625".
BallnoseVcarve.png


Specify a flat depth. This limits how deep the bit will go regardless of the angle (or radius for a ballnose bit).
Image

Change the distance between the vectors. If the vectors are closer together the bit won't go as deep.
- Randall Newcomb
User avatar
Rcnewcomb
Vectric Wizard
 
Posts: 3568
Joined: Fri Nov 04, 2005 5:54 am
Location: San Jose, California, USA
Model of CNC Machine: GCnC/WinCNC


Return to Post Processors

Who is online

Users browsing this forum: No registered users and 3 guests