Machsupport Forum

Mach Discussion => General Mach Discussion => Topic started by: josh on June 07, 2010, 12:36:32 AM

Title: Tool radius not less than arc radius
Post by: josh on June 07, 2010, 12:36:32 AM

can someone explain to me what do this mean (Tool radius not less than arc radius)
thats what comes up on the STATUS of my screen and also stops my machine form doing the part.

Title: Re: Tool radius not less than arc radius
Post by: M250cnc on June 07, 2010, 06:14:27 AM

Quote from: josh on June 07, 2010, 12:36:32 AM

can someone explain to me what do this mean (Tool radius not less than arc radius)
thats what comes up on the STATUS of my screen and also stops my machine form doing the part.

You are making a 50mm square pocket, in the corners you want a 3mm radius "ARC RADIUS" you set the program to run using a tool of 12mm diameter "6mm TOOL RADIUS"

Which is impossible, so you must use a smaller tool

Title: Re: Tool radius not less than arc radius
Post by: ger21 on June 07, 2010, 11:56:21 AM

I believe this only applies when using G41/G42.

Title: Re: Tool radius not less than arc radius
Post by: RICH on June 07, 2010, 03:18:22 PM

I believe this only applies when using G41/G42.
and also relates to the lead in or out thus tool diameter should be smaller like Phil said.

In the context of the program generating the code, I would think it would error, but don't think that is
the case with LazyCam. ( to lazy to find the info in the manual....   ;D )

RICH

Title: Re: Tool radius not less than arc radius
Post by: josh on June 07, 2010, 09:07:06 PM

Quote from: ger21 on June 07, 2010, 11:56:21 AM

I believe this only applies when using G41/G42.
[/
quote]
what do you mean by saying it only applies when using  g41/g42
because I am using g41/g42.
thanks for the replies to everyone.

Title: Re: Tool radius not less than arc radius
Post by: ger21 on June 07, 2010, 09:43:16 PM

You'll only get the error when using G41/G42, because Mach3 can't apply the offset.

Title: Re: Tool radius not less than arc radius
Post by: josh on June 07, 2010, 11:35:23 PM

so what would be your sudggestion for me to fix this problem

Title: Re: Tool radius not less than arc radius
Post by: Sam on June 07, 2010, 11:56:06 PM

1. Use a smaller tool to achieve the programmed radius.
or
2. Use a larger radius in the program.
or
3. Use a combination of both 1 and 2.
or
4. If caused by to short of a lead-in, increase the lead-in distance.

There are a few scenarios that you would get this error. As stated above, it could be caused by to short of a lead-in when applying the tool comp. It could also be caused by a bad choice of tool diameters, or to small of a fillet radius in the part program. If you could post your code, and tell us what cutter your using, we could get a better understanding of what's going on.

Title: Re: Tool radius not less than arc radius
Post by: ger21 on June 08, 2010, 06:36:47 PM

Assuming it's not a lead in issue, basically, just make sure any inside corners have a radius larger than the tools radius. That's it.