First Sign Carve - "V" Bit - Problems

This forum is for general discussion regarding VCarve Pro
User avatar
adze_cnc
Vectric Wizard
Posts: 4327
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: First Sign Carve - "V" Bit - Problems

Post by adze_cnc »

blackte wrote:I have run several things before without any issues...
Do you have a sample CRV file of something that has run properly in the past as comparison to to this file?

Steven

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: First Sign Carve - "V" Bit - Problems

Post by Leo »

YEP

You are telling V-Carve that Z zero is top of material

BUT - BUT

You are telling the machine that Z Zero is the machine bed

SOOO - V-carve posts out a program --- THINKING that Z zero is top of material. It drives the tool to zero which is in fact the machine bed. The machine did what it was supposed to do.

You either need to tell the machine that the zero is the top of material OR - select the bottom of material in V-Carve. ONE - or the other.

This is why I was asking you HOW you set zero in your machine.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

blackte
Vectric Apprentice
Posts: 72
Joined: Thu Nov 01, 2018 1:40 pm
Model of CNC Machine: NewCNC Talent T2

Re: First Sign Carve - "V" Bit - Problems

Post by blackte »

Yep, just looked at another one that I did, and Machine Bed was checked. I guess I screwed up. Not the first nor will be the last. I was thinking I had seen in one of the tutorial video's if you are carving, you need to set the "Z" to top of material. Once I get my machine re-set, I will try it again to see what happens. Sometimes it's the smallest things to cause you many headaches. I will repost the outcome once I get the file to run again.

Thanks to all for your input.

ger21
Vectric Wizard
Posts: 1592
Joined: Sun Sep 16, 2007 2:59 pm
Model of CNC Machine: Custom DIY
Location: Lake St Clair, MI, USA
Contact:

Re: First Sign Carve - "V" Bit - Problems

Post by ger21 »

If the material thickness varies, it's often better to set Z zero to the top.

But then you would need to set Z zero at the top on your machine, and my guess is that it's not easy to do that, if at all?
Gerry - http://www.thecncwoodworker.com

User avatar
Leo
Vectric Wizard
Posts: 4082
Joined: Sat Jul 14, 2007 3:02 am
Model of CNC Machine: 1300 x 1300 x 254 Chinese Made
Location: East Freetown, Ma.
Contact:

Re: First Sign Carve - "V" Bit - Problems

Post by Leo »

Not a problem at all.

Been there done that and WILL most certainly be doing it again and again.

Glad we could help.

BTW - that machine looks like a nice beefy machine.
Imagine the Possibilities of a Creative mind, combined with the functionality of CNC

blackte
Vectric Apprentice
Posts: 72
Joined: Thu Nov 01, 2018 1:40 pm
Model of CNC Machine: NewCNC Talent T2

Re: First Sign Carve - "V" Bit - Problems

Post by blackte »

Leo - yes it is. It is quick and powerful. It will cut just about anything including solid surface material. My main focus is cabinets and doors. I have just started messing around with carving and signage. Trying to add some unique items to my business.

That is one thing I really like about this forum, everyone is very helpful. I belong to other forums and they are not even close to this one. I can spend hours looking through posts just to gain knowledge about what others are doing and the problems they are running into. It's so helpful.

ezurick

Re: First Sign Carve - "V" Bit - Problems

Post by ezurick »

Wow! brings back memories... I had that happen to me a couple of times. It was always user error. First time it happened, I zeroed xyz for my material, then loaded in the vcarve .txt to mach3 and hit start and ... blame. Here mach3 decided to CHANGE my xyz to some astronomical number after I loaded in the file and I didn't notice it. I now zero AFTER I load in the file. lol.

That said... if he was getting decent cuts with circles using same settings, why would it be different now? However, I agree that the LENGTH of the tool should be immaterial. I am unfamiliar with his machine, but it does sound like he is not setting the zero to the top of the material properly.

User avatar
TReischl
Vectric Wizard
Posts: 4596
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: First Sign Carve - "V" Bit - Problems

Post by TReischl »

blackte wrote:Here are my settings for this CRV file. To me this is correct. It has the material as 3/4" thick and "Z" is top of material.
No. You said that the machine knows where the surface of the table is at.

Absolutely none of your Z moves should have a negative Z value unless you want to cut into your spoilboard/machine bed.

Here is what your code should look like:

M3
N7 G00 X-13.0397 Y-1.3058
N8 G00 Z1.5000
N9 G00 X-13.0397 Y-1.3058
N10 G00 Z1.1000
N11 G1 X-13.0397 Y-1.3058 Z0.8750 F100.0
N12 G1 X-14.1247 Y-1.3058 Z0.8750 F300.0
N13 G1 X-14.1247 Y-2.3908 Z0.8750


The only way this would not be correct is if you somehow entered material thickness into the machine control.

The above file is based on a part 1 inch thick.
"If you see a good fight, get in it." Dr. Vernon Johns

Post Reply