Does anyone use Vcarve Pro?

Discuss Thermwood 3-axis Machinery, Controller, and Software.

Moderators: Jason Susnjara, Larry Epplin, Clint Buechlein, Rich Kasten

Joshua Eller
New Member
Posts: 6
Joined: Mon, Jun 15 2015, 9:39AM
Company Name: Robertson Furniture
Country: UNITED STATES

Does anyone use Vcarve Pro?

Postby Joshua Eller » Mon, Jun 15 2015, 10:28AM

Hello everyone, My company recently purchased Vcarve Pro and its a really nice software for the price. My problem is cutter radius compensation. If I were there with the machine as I was programming it probably wouldn't be such a big deal but we really dont want to have to regenerate a program everytime we change a bit because we constantly use re-sharpened tools. Our machine uses the 91000 super control and the post processor for that control in vcarve only posted G1 codes for everything but I modified it to post G2/G3 codes as well. That being said I also added a couple things to allow a G42 at the plunge line and a G40 at the retract line. so far this seems to be working but I feel like this is a band-aid for the issue rather than a solution. Do you guys have this problem? Any suggestions for handling this? Attached below is the post I have modified.
Attachments
Thermwood_ATC_91000_ARCS_inch_G42.txt
Here is the post I have modified.
(5.04 KiB) Downloaded 108 times

Joshua Eller
New Member
Posts: 6
Joined: Mon, Jun 15 2015, 9:39AM
Company Name: Robertson Furniture
Country: UNITED STATES

Re: Does anyone use Vcarve Pro?

Postby Joshua Eller » Mon, Jun 15 2015, 10:58AM

I should also add, the way I use this post is I nest the parts in the program, using a profile cut, I specify outside profile with a conventional cut and have the tool diameter set to .001" this gives a .0005 radius offset to the tool path but we're cutting wood parts here so its not aerospace critical to be that accurate.Then to allow the control to compensate, that is where the G42 comes into play.

Daniel Odom
Senior Member
Posts: 204
Joined: Thu, Oct 20 2011, 12:52PM
Company Name: Carlton Kitchen and Bath
Country: UNITED STATES

Re: Does anyone use Vcarve Pro?

Postby Daniel Odom » Mon, Jun 15 2015, 12:23PM

Cool, I thought about doing this before but never had enough time to get around to it. I just try to not use resharpened tooling except for one changer position that I use specifically for the expensive 3/8" resharpened compression bits or down spirals; and I only used that for one off jobs that I don't need to re-post. Everything else I just use up and throw away (mostly 1/4" and 1/8"), not worth the hassle and risk of having a pallet of wrong parts that you don't find out about until after the shop guys start assembling.

Joshua Eller
New Member
Posts: 6
Joined: Mon, Jun 15 2015, 9:39AM
Company Name: Robertson Furniture
Country: UNITED STATES

Re: Does anyone use Vcarve Pro?

Postby Joshua Eller » Mon, Jun 15 2015, 1:30PM

I know what you mean, if we used smaller bits I would probably do the same thing but we use a 3/8" compression bit about 80% of the time and a range of others from 1/2" to 3/4", all of the bits we use are carbide and a few diamond tipped as well so it would be very costly for us to toss those after use.

User avatar
Josh Rayburn
eCabinets Beta Tester
Posts: 1262
Joined: Wed, Jul 01 2009, 2:19PM
Company Name: Halls Edge Inc
Country: UNITED STATES
Location: Stamford, CT USA
Contact:

Re: Does anyone use Vcarve Pro?

Postby Josh Rayburn » Tue, Jun 16 2015, 9:34AM

Hi Joshua,
I think the G41 / G42 cutter compensation is the only possible solution if you are unable to post with a known tool diameter. Sounds like you're on the right track already for whatever that's worth. We have been using VCarve Pro for a while, and we are delighted with it.
jnr
Josh Rayburn
Hall's Edge, Inc.
CNC Machining Service


Dell Precision T3400
Win7 Professional 64 Bit/Core2Duo E8400 3ghz/4 GB Ram/NVIDIA Quadro FX570

Joshua Eller
New Member
Posts: 6
Joined: Mon, Jun 15 2015, 9:39AM
Company Name: Robertson Furniture
Country: UNITED STATES

Re: Does anyone use Vcarve Pro?

Postby Joshua Eller » Tue, Jun 16 2015, 9:53AM

Thanks Josh, I appreciate the feed back. I really like the software and its features especially for the price of it. Like I said I feel like the modifications to the post I have made are only temporary fixes. I have made a couple different PP to handle a few different situations I come across based on the particular machining strategy needed at the time. I am mostly just not sure if I the way I have it setup is the correct way of posting the code. So far I have not had any issues with cuts and all the parts are spot on as far as dimensions. Fingers crossed, I hope it continues to work for us and maybe Vectric will implement cutter radius comp in the near future......

David Egnoski
Senior Member
Posts: 184
Joined: Tue, May 17 2005, 1:05PM
Company Name: Richmond Cabinet
Country: UNITED STATES
Location: Delavan, WI

Re: Does anyone use Vcarve Pro?

Postby David Egnoski » Fri, Jun 26 2015, 7:19AM

Contacted Vectric about radius comp. They have no plan to add this feature.

Josh,
How do you handle radius comp? I have VCarve jobs that I have been running for the past 3 years. The parts don't change. Just encountered a fit problem because I switched to a sharpened tool. I've always entered the nominal tool diameter in VCarve. I'm not excited about having to recalculate each time a tool radius changes.

I guess I'm spoiled by the way eCab and Thermwood handle this for me.
Dave Egnoski
Richmond Cabinet & Millwork

Joshua Eller
New Member
Posts: 6
Joined: Mon, Jun 15 2015, 9:39AM
Company Name: Robertson Furniture
Country: UNITED STATES

Re: Does anyone use Vcarve Pro?

Postby Joshua Eller » Fri, Jun 26 2015, 7:46AM

David Egnoski wrote:Contacted Vectric about radius comp. They have no plan to add this feature.

Josh,
How do you handle radius comp? I have VCarve jobs that I have been running for the past 3 years. The parts don't change. Just encountered a fit problem because I switched to a sharpened tool. I've always entered the nominal tool diameter in VCarve. I'm not excited about having to recalculate each time a tool radius changes.

I guess I'm spoiled by the way eCab and Thermwood handle this for me.



So far with the modified PP I have made, I havent had any issues with CRC yet and part fitment has been spot on. That being said, this only works with a profile cut using conventional cutting and set the tool diameter to .001, I have a two of the most common used tools in the tool manager setup, one with the actual dia. and one with the .001 dia. that way if i have to cut a pocket for a fixture or something I can just post that tool path alone and then past it in the compensated post to keep it all one file. If we do a vcarve tooling path I still have to measure the tools and let vcarve calulate the tool path itself or else the tool path is way off. One thing I have done was created a few different PP to handle different situations. I have one with a G42 and one with a G41 and one with neither. I will attach the PP I have modified, you will have to set them up for your machine offsets and such but maybe it will help a little. You will have to take off the .txt extension to get vectric to read it.
Attachments
Thermwood_ATC_91000_ARCS_inch_G42.pp.txt
This one is the what I use most.
(5.51 KiB) Downloaded 91 times
Thermwood_ATC_91000_ARCS_inch_G41.pp.txt
(5.08 KiB) Downloaded 96 times
Thermwood_ATC_91000_ARCS_inch.pp.txt
This one has no cutter radius compensation at all.
(4.93 KiB) Downloaded 104 times

David Egnoski
Senior Member
Posts: 184
Joined: Tue, May 17 2005, 1:05PM
Company Name: Richmond Cabinet
Country: UNITED STATES
Location: Delavan, WI

Re: Does anyone use Vcarve Pro?

Postby David Egnoski » Fri, Jun 26 2015, 9:05AM

Joshua,
Thanks for posting your PP.

The jobs I'm cutting would require G41 and G42 in the same job. Parts are nested inside parts. Not sure how that would be implemented.

FYI
Vectric's guide for modifying PPs says all commands should be in double quotes.
Dave Egnoski

Richmond Cabinet & Millwork

Joshua Eller
New Member
Posts: 6
Joined: Mon, Jun 15 2015, 9:39AM
Company Name: Robertson Furniture
Country: UNITED STATES

Re: Does anyone use Vcarve Pro?

Postby Joshua Eller » Fri, Jun 26 2015, 9:17AM

David, One thing I have done is selected the paths that I wanted to post with a G41, calculate those then the paths I wanted G42 and calculate those since vectric lets you post tool paths separately, I post the the paths with the PP G41 or G42 then copy them into the same file, maybe this helps a little?


Return to “Thermwood 3-Axis Machinery”

Who is online

Users browsing this forum: No registered users and 1 guest