profile tool path vs. V acrve tool path

This forum is for general discussion regarding VCarve Pro

profile tool path vs. V acrve tool path

Postby raye321 » Sun Jul 01, 2018 12:30 am

Hi, I'm working on a project and trying different tool paths to see which will work best. At first, I wanted to use the v carve tool path feature for the project. But I couldn't get it to work for me. I couldn't get the bit to cut to the depth I entered, or any depth. It stayed above the work piece, barely touching. So I tried the profile tool path feature. Same bit, 60% .5" dia. It worked fine. The project looks good. I have been using the v carve pro 8.5 and 9.0 for over a year. I always used the quick engrave feature using an end mill bit to fill or outline. My question is: what is the main difference between using a v bit with the profile tool path or v carve tool path? What does the v carve feature do that the profile feature doesn't?
Thank you
raye321
 
Posts: 12
Joined: Thu Feb 02, 2017 3:08 pm
Model of CNC Machine: Digital Carver

Re: profile tool path vs. V acrve tool path

Postby 4DThinker » Sun Jul 01, 2018 12:49 am

The Vcarve toolpath require a closed shape. It changes depth depending on how far apart the side of the shape are.
The Profile toolpath follows a vector, and gives you the choice of cutting inside, outside, or ON the vector.

You might look into the fluting toolpath if you want to follow a vector. It can slope down to your set depth at the beginning and slope up at the end of a vector.

4D
4DThinker
Vectric Wizard
 
Posts: 1115
Joined: Sun Sep 23, 2012 12:14 pm
Model of CNC Machine: CNC Shark Pro

Re: profile tool path vs. V acrve tool path

Postby Adrian » Sun Jul 01, 2018 8:42 am

Did you redraw the vectors as suggested in your previous post? The vectors were really poor quality so I wouldn't be surprised that you couldn't get the V-Carve toolpath to work. What looks like a nice, neat shape to the human eye at a normal scale often isn't when you zoom in which was your problem with the file you posted.

The profile toolpath and V-Carve toolpath are radically different toolpaths. The only time you'll get similar results is if you're v-carving closed vectors with a constant, close gap between them. A circle within a circle offset by a 1/16" or so will give a toolpath result that looks pretty much identical to a profile toolpath with the same tool because the v-carve toolpath is maintaining a constant depth as it's "rides" the vectors. Now increase the gap between the circles to an inch or make one of them a square and you're get very different results.
User avatar
Adrian
Vectric Archimage
 
Posts: 8349
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: profile tool path vs. V acrve tool path

Postby sharkcutup » Sun Jul 01, 2018 5:25 pm

V-bit test.png


Bit used --- 60 degree .5 diameter by .625" cut height V- Bit Database settings -- .5 dia. 60 degree 0.125 pass depth

First line text - Profile Tool Path at .02 flat cut depth Machine Vectors --- ON

Second line text - V-Carve Tool Path at .02 flat cut depth

Third line text - V-Carve Tool Path NO Depth set other than database setting of 0.125

Fourth line text - V-Carve Tool Path Tried to force flat depth to .5" but as you can see it is cut at about the same depth as the third line text which leads me to believe that the v-bit will tend to stay at a comfortable depth within the vectors boundary.

Fifth line text - V-Carve Tool Path Text Vectors moved outwards 1/16"and kept the .5" flat depth which thereby achieved that depth in a couple of the letters (h, e)

In the above test which all text are CLOSED vectors at a determined sustained width
In a Profile Tool Path ON the vectors at shallow depths will provide an acceptable tracing of the text -- but if you go too deep (this ex: 0.15") they become unacceptable (Looking more like line five text)

In a V-Carve Tool Path all material in between the closed vector will be carved at a depth (a - sustained by the distance of the narrow closed vectors or b - a flat depth set by user that is reasonably and consistently acceptable to maintain clear and defined text characters.)

Hope this makes sense and helps!!!


Sharkcutup
Facebook: Hogan's CNC Crafts
Website: hoganscnccrafts.com
V-Carve Pro 9.508
sharkcutup
Vectric Craftsman
 
Posts: 211
Joined: Sat Mar 26, 2016 3:48 pm
Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle

Re: profile tool path vs. V acrve tool path

Postby adze_cnc » Sun Jul 01, 2018 7:19 pm

what is the main difference between using a v bit with the profile tool path or v carve tool path?


Have you read the help file? It's all explained there. https://docs.vectric.com/docs/V9.0/VCarvePro/ENU/Help/Home.html
User avatar
adze_cnc
Vectric Apprentice
 
Posts: 440
Joined: Sat Jul 27, 2013 10:08 pm
Location: Vancouver, BC, Canada
Model of CNC Machine: AXYZ 4008

Re: profile tool path vs. V acrve tool path

Postby ger21 » Sun Jul 01, 2018 8:46 pm

Fourth line text - V-Carve Tool Path Tried to force flat depth to .5" but as you can see it is cut at about the same depth as the third line text which leads me to believe that the v-bit will tend to stay at a comfortable depth within the vectors boundary.


The flat depth setting will restrict the depth to the flat depth, so if the depth from normal V carving is less than the flat depth, it will have no effect.
Flat depth is most often used on larger letters and shapes, where normal v-carving would cut too deep.
Gerry
ger21
Vectric Wizard
 
Posts: 1143
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA

Re: profile tool path vs. V acrve tool path

Postby raye321 » Mon Jul 02, 2018 7:15 pm

Thanks for the helpful info guys,
Yes I did redo the drawing I had. It came out better.
raye321
 
Posts: 12
Joined: Thu Feb 02, 2017 3:08 pm
Model of CNC Machine: Digital Carver


Return to VCarve - General

Who is online

Users browsing this forum: ozymax and 19 guests