Radius Compensation

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

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

Kim Dang
New Member
Posts: 2
Joined: Mon, Jan 25 2016, 6:31PM
Company Name: Mart Design
Country: CANADA

Radius Compensation

Postby Kim Dang » Sat, Mar 26 2016, 9:30AM

Hi all,
I have 58 letters nested on 1 sheet.When I nested the job, no errors or warnings appeared. The nesting was fine, but the cut. When it cut for a bout 20 minutes, the machine stopped and the window said " while radius compensation is one, a line to arc intercept calculation failed" I tried to re-nested and re-cut the job. Same thing happened at the same place. I searched for solutions from the forum. I reduced .001" from the tool diameter and re-cut the job. Same error appeared. I tried and tried 5 times on the same sheet until midnight. Tired of waiting 20 mins before the machine stops each time I try to recut. Could you plz tell me if I can start the job where it stopped before?
Look forwards to your reply
Thanks

Forrest Chapman
eCabinets Beta Tester
Posts: 1091
Joined: Mon, May 30 2005, 2:26PM
Location: Anderson SC.
Contact:

Re: Radius Compensation

Postby Forrest Chapman » Sat, Mar 26 2016, 12:36PM

You may be able to move a few lines down and start from there. It might be that it leaves a little geometry to clean up by hand but that is better than not getting the job done. Can you post the file you are trying to cut?

Forrest

User avatar
Kerry Fullington
Wizard Member
Posts: 4566
Joined: Mon, May 09 2005, 7:33PM
Company Name: ProSource of Amarillo
Country: UNITED STATES
Location: Amarillo, TX

Re: Radius Compensation

Postby Kerry Fullington » Mon, Mar 28 2016, 12:33PM

Kim,

I had a similar problem once and mine was caused by a curved part that tapered to absolutely nothing. I had to take my file into Contour in the Part Editor and did a small (.0625) filet so the part didn't go to nothing. This allowed the machine to think it could make the turn.

Look at your drawing where the machine stops and see what your parts look like.

User avatar
Josh Rayburn
eCabinets Beta Tester
Posts: 1261
Joined: Wed, Jul 01 2009, 2:19PM
Company Name: Halls Edge Inc
Country: UNITED STATES
Location: Stamford, CT USA
Contact:

Re: Radius Compensation

Postby Josh Rayburn » Wed, Mar 30 2016, 6:28AM

Kim,
I get that all the time. I just find the J or I coordinate that is a 0 and change it to anything other than 0 and it works great.
Also, once you start the file and complete the first tool change, you can navigate to another tool change, or if you already have the tool you want, then you can navigate anywhere in the code and press start. You will probably get a confirmation "are you sure you want to start here?" just say yes and you're back where you left off.
Hope this helps,
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

Dave Burtchell
Junior Member
Posts: 98
Joined: Thu, Jun 30 2005, 10:04PM

Re: Radius Compensation

Postby Dave Burtchell » Fri, Apr 01 2016, 1:31PM

We've had this problem for years. In our case, it stems from the fact that our cad software, Rhino, outputs the dxf file in 8 decimal places, while Thermwood only reads 4. The fourth decimal place is either rounded up or down depending on Rhino's 5th decimal. So, when we get the "line to arc intercept" error, we look at the g-code line that's highlighted, and the next line down. That second line of code usually has either an "x", or "y" value that is .0001" higher or Lower than the highlighted line. Let's say the highlighted line is y23.1234 and the next line is y23.1235, or y23.1233. We hit "tab" and change the first line to match the second line and continue on. Works for us every time now. We used to agonize over a workaround, or redraw the part, or skip ahead and forget the bad part. Try it, you'll like it. Let us know if the explanation isn't clear.

Dave


Return to “Thermwood 3-Axis Machinery”

Who is online

Users browsing this forum: No registered users and 4 guests