Giant radius get posted as linear not circular moves?

[Snaglpuss]

Hi All,

Got a job that has some giant radiuses or radi?

Like 250 feet +/- anyway when posting the parts

the code comes up as linear G1 moves not arc moves.

Parts seem to be ok, but is their some certain size limit to arcs that gets them to "linearize" and not post as arc moves?

[Guest]

if you're using filter make sure the upper end of the filter size will accommodate your arc size

[Chris Parish]

no arc can be larger than 99 inches.. other wise it is considered linear

[Troy Gossett Indepak Inc.]

When you backplot are you seeing the linear segements? If not it is most likely your post. There is a line something like " Forces output of I,J,K arc centers (arcoutput:0 " for more info check the helpfile.

 

CParish. Where did you find a limit on arc size? It seems Aerospace makes many parts with tight tolerances that would be much larger than 99"

[Chris Parish]

oop ... nice catch 999 inches...

[Jim Evans from CNC Software]

If there is an Arc in the NCI then the post is linearizing it. If there is no arc in the NCI and only linear moves in it's place then the toolpath is linearizing it.

 

There is a min and max arc radius tolerance that MP/Posts will use in the Control Definition under the tolerances topic. There is also a Min/Max arc radius int he Arc Filter/Tolerance topic in your toolpath that Mastercam will use when creating arcs via the filter.

 

Check both of these tolerances to ensure your settings allow for your desired arc size.

[Snaglpuss]

Thanks for the quick answers.

 

My arc limit has to be way greater than 99 inches,

we do woodwork and use fairly large arcs all the time. Just never noticed them posting to lines before.

 

Can't find arcoutput:0 type command in the post,

what section of the post would that be in?

 

Looked in the control definition and found my limit set at 999.9999.

 

Where is the "Arc Filter/Tolerance topic in your toolpath" located?

Is there any problem setting it to a higher number

or is that the limit?

 

[ 06-09-2009, 03:36 PM: Message edited by: Snaglpuss ]

[Guest CNC Apps Guy 1]

 

In the control definition, the three settings that are circled work together.

[Snaglpuss]

Thanks, but what happens if I increase my arc limit or is there a max that MC supports? Or is it dependent on the physical machine?

[Jim Evans from CNC Software]

Sorry for the confusion but I've been stuck in X4 for a while now. The Arc Filter / Tolerance topic is in the X4 interface.

 

In the X3 interface there is a Filter button on the toolpath parameters page located just under the Lead in/out button on the lower right side. Tick the check box on and click to the button to display the filter settings dialog

[Guest CNC Apps Guy 1]

Those values should be set to your machine's limits. You may need to consult your machine builder for that info. The settings in Mastercam are pretty generic to work with the maximum number of machine tools.

[Scott Lundin Shopware Inc.]

I have had a few machines that take off in unexpected ways when it sees an arc larger than 99.9 inches. Be attentive with feed hold and rapid reduce on the first part! (Mazak Vari-axis 630, Matrix control for one)

[Snaglpuss]

Thanks to all responders.

[88Matt]

If all else fails I guess you could convert it to a spline and cut.

[john316]

.

 

quote:

---

Those values should be set to your machine's limits.

---

This is a big factor here. Your machine has a max radius limit and will either take off or alarm out. You should be able to find the machine's arc limit in your Operator's manual. If you can't get the arc you need you'll have to use a spline and run it point to point.

 

.