Hello Guest it is October 19, 2019, 04:07:29 AM

Author Topic: Arc Radius and cutter radius  (Read 4172 times)

0 Members and 1 Guest are viewing this topic.

Offline Psad

*
  •  82 82
    • View Profile
Arc Radius and cutter radius
« on: December 23, 2006, 08:54:21 AM »
I'm not really sure if this is related to LC, Gcode or Mach3 so i'm starting here.
I'm trying to cut an inside pocket.  Autocad readuis is set for .0625, Cutter tool diameter is .125" (tool #2).
When i get to the first inside corner (around n265) i get the following errror and cannot proced.
"tool raduius not less that acr radius with como on line number......"

I've tried setting the tool diameter to .120" but i still get the error.
do i have to reload from LC when i chage the tool size on the fly.

attached are the two files can someone tell me what i'm doing wrong.

Also I cannot really read the entire message, the line number is cut off.
suggest that you replace "less than" with "<" and "number" with "#"  in that message to complete display in the space given.

As always folks thanks in advance
Re: Arc Radius and cutter radius
« Reply #1 on: December 23, 2006, 09:14:07 AM »
The inside Rad must be greater then the tool rad, they can't be the same :(
Fixing problems one post at a time ;)

www.newfangledsolutions.com
www.machsupport.com

Offline Psad

*
  •  82 82
    • View Profile
Re: Arc Radius and cutter radius
« Reply #2 on: December 23, 2006, 09:55:57 AM »
Thanks Brian - My assumption is Mach3 would just cut make a square move if they were the same but wouldn't changing tool #2 from .125 to .120 have addressed that problem.

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Arc Radius and cutter radius
« Reply #3 on: December 24, 2006, 11:28:36 AM »
I set my tool #2 to .12 and it worked fine. Are you using the lat3est version. 1.84 has some comp bugs. Also, do you have advanced comp turned on?
« Last Edit: December 24, 2006, 11:36:43 AM by ger21 »
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Arc Radius and cutter radius
« Reply #4 on: December 24, 2006, 11:57:09 AM »
Hi there,
I am new here so I need to tell you a bit about my self. Iam a independend contractor that does al the training for Bobcad. I also own a machine shop where we make custom parts for motorcycles, hot roads and so on. I have Mach 2 on one of my old mills that I didn't wanted to part with it. I use the Fanuc post processor and it works fine for me (I will try to set one up just for Mach and when I do that, I will post it here). Anyway, My post outputs after each H value a D value that always matches the tool number and height (tool lenght\G43). That way when a tool change is made and the TL is picked up, the controll also knows the tool diemater. If you don't use the D value, it is possible that each time you will be using G41/G42 it will remember the last value that it has read. Just a heads up, if you have inside corners that are the same value as your tool cutter, you might run into trouble, also using cutter comp. allows you to tweak the size of the part. I will always use a smaller tool then the inside corners so I can adjust the size of my part. Think about this: Thbe inside corners are 125, the tool is .25 dia (.125 rad) and now you need to make the part let's say .002 bigger all around. You will need to lie to the control that tool dia is .252 (.126 rad) so now you are going to get all the cutter comp errors....
Just my 2 cents,
Merry Christmas to you all
Sorin Nenu Cad Cam Trainer
www.cadcamtrainer.com

Offline ger21

*
  • *
  •  6,288 6,288
    • View Profile
    • The CNC Woodworker
Re: Arc Radius and cutter radius
« Reply #5 on: December 24, 2006, 03:07:39 PM »
Sorin, the D is not needed as long as the current tool is correct. The M6 T1 sets the current tool and Mach will use the current tool if no D is specified in the G42. I also thought that was the problem, but simulated it in Mach3 and saw that it worked fine.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Arc Radius and cutter radius
« Reply #6 on: December 24, 2006, 04:26:29 PM »
Ger,
Thank you for letting me know about that because I was starting a new post processor to be use with Bobcad and wasn't aware of it. I always had the H and D on my line (perhaps too familiar with the Fanuc and Haas controlers). Anyway, a D word in the same line as the G41/G42 will allow the user to use 2 different d offsets for the same tool for semifinish and finish passes. I use that all the time where I use D 21 to semifinis a part  (I add about .005 to the tool dia there) and D 1 for finish path (corect tool dia). That will be for T1  and so forth.
Merry Christmas!
Sorin Nenu Cad-Cam Trainer
www.cadcamtrainer.com