post tool radius dosn't align

[deanj]

I'm using a Haas VF4 machine. While doing a prerun I received an alarm(302 for you Haas users). The alarm indicated ther was an invalid radius in my "G02" or clockwise interpolation motion.

The discription of the alarm tells me to check my geometry, that my radius must be greater or equal to half the distance fropm start to end within a accuracy of .0010 inches.

 

Heres where my code goes all wrong -

X1.8446 Y3.7283 R.375

X2.2146 Y5.5501 R.375

 

I'm pretty sure the problem is some kind of tolerance setting in Mcam, I,ve already tried changing my post processor settings from R to I,J that didn't work.

Any assistance would be greatly appreciated.

Thanks..JMD...

[Roger Martin from CNC Software]

quote:

---

I'm pretty sure the problem is some kind of tolerance setting in Mcam,

---

Probably not, unless you have altered the default intsall tolerances. More information would be required to be able to assist. The two blocks shown look fine, but want is the X,Y position PRIOR to the first arc move? Take that location and draw it in MC. Then draw the X,Y arc endpoints and the arcs based on the NC code coordinates. Does this look like it should be "good" motion? Also, are you running comp in control ? If so, how much comp is in effect, offset to which side on these arcs?

[Guest CNC Apps Guy 1]

Something else, if you are using comp in control, you'll need to make sure you have a lead in line that is greater than the value of compensation you are putting in at the control.

 

I personally prefer to use wear compensation (Left/Right in computer AND Left/Right in control). This meant that you will put the difference between the programmed radius/diameter of the tool and actual radius/diameter. I NEVER have problems unless I forget to put that lead in line in.

 

Hope that helps.

[Surface]

The X,Y, Rad circle format you are using can cause problems and I urge you to use the I, J format. Rounding of the radius values which naturally occurs can cause some extreme errors.

To prove this, create/arc/circ pt+rad. Enter value of 1" radius and center on the origion. Next Trim the circle to yeild a half circle. Now, create/arc/endpoints. Choose the endpoints from the previous arc and enter a value of 1.0001 radius. You will find the circle is more than .014 out of round by the .0001 difference in radius.

I doubt this will fix your problem, but I am sure it will save you some head-skrachen someday.

[RandyN]

If you haven't done so, installing then latest post exe fixed a similar problem we were having.