Cutting lower then flat depth

This forum is for general discussion regarding VCarve Pro
Post Reply
User avatar
Makingtoothpicks
Vectric Apprentice
Posts: 512
Joined: Tue Jul 23, 2013 8:46 pm
Model of CNC Machine: Cncrouterparts CPR2448
Location: Burien, Wa
Contact:

Cutting lower then flat depth

Post by Makingtoothpicks »

I am working on a project. I cut out a pocket to a depth of .125.
I then want to Vcarve some text in the pocket. If I set the Start
at .125 and use the Vcarve and no flat it cuts to .1641. I want
to carve the text to a depth of .125. So I set a flat depth of .125
run the TP and it still cuts the text to .1641. I am using a 90 deg
V bit. I know I am doing something wrong. Do I need to use a
bit with a flat tip defined

Thank You
Don.

User avatar
dealguy11
Vectric Wizard
Posts: 1663
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA
Contact:

Re: Cutting lower then flat depth

Post by dealguy11 »

If you set the start depth to .125", with no flat depth, it cuts to .1641". That means the v-carve path is cutting .0391" into the material. When you set the flat depth to .125, it doesn't make a difference because the toolpath never cuts .125" deep. For the flat depth to make a difference, the initial cut would have had to go deeper than .25".
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com

User avatar
dealguy11
Vectric Wizard
Posts: 1663
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA
Contact:

Re: Cutting lower then flat depth

Post by dealguy11 »

I'm not sure that was clear. Here's a diagram that hopefully illustrates what I think is happening.
Attachments
Depths.JPG
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com

User avatar
Makingtoothpicks
Vectric Apprentice
Posts: 512
Joined: Tue Jul 23, 2013 8:46 pm
Model of CNC Machine: Cncrouterparts CPR2448
Location: Burien, Wa
Contact:

Re: Cutting lower then flat depth

Post by Makingtoothpicks »

I am sorry I did not state the settings correctly .Pocket depth .125
Start depth .125
Flat depth .250
even with these settings it is cutting the text at .1641.
I thought I would get text cut to .125 depth.


Don

User avatar
adze_cnc
Vectric Apprentice
Posts: 1065
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Cutting lower then flat depth

Post by adze_cnc »

Perhaps you should read the help file again. The flat depth is relative to the start depth. It is not an absolute depth from the top of the material.

Given all this dealguy's image and posts still hold true.

User avatar
dealguy11
Vectric Wizard
Posts: 1663
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA
Contact:

Re: Cutting lower then flat depth

Post by dealguy11 »

I'm going to give this one more shot.

If you had zero start depth and zero flat depth, I'd be willing to bet that your v-carve toolpath would only cut 0.0391" deep. This is controlled by the angle of your v-carve bit and the distance between the parts of the closed vector you are using to define the v-carve toolpath.

I you were to take this path, with 0 start depth, and change the flat depth to 0.125", then nothing would change. You'd still only cut 0.0391" deep because it only uses the flat depth when the flat depth is less than how deep the bit would cut without it. Since 0.0391" is less than 0.125", you do not get a flat.

When you add a 0.125" start depth, then the bit cuts .1641" deep because it is adding the .125" start depth to the 0.0391" the bit cuts into the material.

If you add a 0.125" flat depth to the start depth above, then nothing will change, because 0.125 + 0.125 = 0.25", which is deeper than the bit is currently cutting (0.1641"). You would only get a flat if the start depth plus the flat depth was less than 0.1641"

Does that help?
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com

User avatar
martin54
Vectric Wizard
Posts: 5185
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber System 48,Denford Triac Modified
Location: Crossgates, Scotland

Re: Cutting lower then flat depth

Post by martin54 »

Or to put it another way Don if you want to cut the text to exactly 0.125 deep then the vcarve toolpath is not the correct toolpath to use :lol: :lol:

Is there a particular reason you want the text at that depth?

User avatar
Makingtoothpicks
Vectric Apprentice
Posts: 512
Joined: Tue Jul 23, 2013 8:46 pm
Model of CNC Machine: Cncrouterparts CPR2448
Location: Burien, Wa
Contact:

Re: Cutting lower then flat depth

Post by Makingtoothpicks »

dealguy11 wrote:
Sat Jul 18, 2020 3:52 am
I'm going to give this one more shot.

If you had zero start depth and zero flat depth, I'd be willing to bet that your v-carve toolpath would only cut 0.0391" deep. This is controlled by the angle of your v-carve bit and the distance between the parts of the closed vector you are using to define the v-carve toolpath.

I you were to take this path, with 0 start depth, and change the flat depth to 0.125", then nothing would change. You'd still only cut 0.0391" deep because it only uses the flat depth when the flat depth is less than how deep the bit would cut without it. Since 0.0391" is less than 0.125", you do not get a flat.

When you add a 0.125" start depth, then the bit cuts .1641" deep because it is adding the .125" start depth to the 0.0391" the bit cuts into the material.

If you add a 0.125" flat depth to the start depth above, then nothing will change, because 0.125 + 0.125 = 0.25", which is deeper than the bit is currently cutting (0.1641"). You would only get a flat if the start depth plus the flat depth was less than 0.1641"

Does that help?
That is very clear. I now know what I need to do. Thank You

Don

User avatar
Makingtoothpicks
Vectric Apprentice
Posts: 512
Joined: Tue Jul 23, 2013 8:46 pm
Model of CNC Machine: Cncrouterparts CPR2448
Location: Burien, Wa
Contact:

Re: Cutting lower then flat depth

Post by Makingtoothpicks »

martin54 wrote:
Sat Jul 18, 2020 5:10 am
Or to put it another way Don if you want to cut the text to exactly 0.125 deep then the vcarve toolpath is not the correct toolpath to use :lol: :lol:

Is there a particular reason you want the text at that depth?
Yes because I need the pocket and the text goes in the pocket. Thank you for your answer.

Don

User avatar
martin54
Vectric Wizard
Posts: 5185
Joined: Fri Nov 09, 2012 2:12 pm
Model of CNC Machine: Gerber System 48,Denford Triac Modified
Location: Crossgates, Scotland

Re: Cutting lower then flat depth

Post by martin54 »

Sorry Don what I meant was does the text need to be 0.125 deep, I understand it needs to go in the pocket. :lol: :lol: If you think it is to bold is it possible to use a different font? I tend to use font families a lot because you get just about every variation of the font you can think of. Might be more difficult to find on free font sites but might be worth a look :lol: :lol: :lol:

sharkcutup
Vectric Wizard
Posts: 917
Joined: Sat Mar 26, 2016 3:48 pm
Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
Contact:

Re: Cutting lower then flat depth

Post by sharkcutup »

TEST.png
90 Degree 0.5 Dia x .4375 cutting depth V-Bit

In this image is two texts in the bottom of a.125" pocket

The first is carved using .125 Start Depth(D) with NONE Flat Depth(F)
The Second is carved .125 Start Depth(D) with Flat Depth(F) checked and .125 in box

Note: The bottom of the letter/characters/text are flat at their bottoms because of the controlled Flat Depth(F)

The first Text Depth is controlled by the angle of bit and the widths of the vectors of the TEXT.

Sharkcutup
www.hoganscnccrafts.com
One on One V-Carve Help is Available!!!
Private Message me for details!

markbachman
Posts: 16
Joined: Thu Jan 05, 2017 2:57 am
Model of CNC Machine: X Carve

Re: Cutting lower then flat depth

Post by markbachman »

Keep in mind that when V carving text the depth of carve is determined by the width of the text.
The narrower the text the shallower the carve.
I suspect your text is not large enough to create a carve .125 deep as you desire.

Post Reply