NX cam - cutting parameters, stock - Intol/Outtol 2

[mechjames]

Hi Guys,
can someone kindly explain the practical use of cutting parameters settings 'Intol' and 'Outtol'. I am making some small parts on the milling machine with reasonable tolerance requirements ideally trying to hold around plus/minus 20 microns. For example I am hole milling a 4.49mm diameter hole on a part with a width of 6mm. Nothing crazy but I would like understand the use of intol and outtol in a case like this. Am I correct in thinking intol represents how much the cutter can go into the material for example if I set this to zero it will not go into the material and outtol is the other side of the tolerance ie how much it can come out? Practically how should I be thinking of the numbers and what sort of values are sensible? Alternatively setting intol positive will set the cutter into the material and outtol zero puts it on the outside edge?

What exactly are these numbers?

What about the 'tolerance' setting inside the model application? Is this effecting the cam? how do I set this for accuracy that is practical?

many thanks,
James

 

[joycejo]

Intol / Outtol will affect the posted output.
If your getting Circular motion G03, G02 the resolution of the machine will control the accuracy.
If your doing some 3-D contouring, Fixed or Variable axis milling, then the Intol / Outtol will make a dramatic difference in the surface finish and length of the program, the moves will be much closer together with a tighter tolerance.

Are you doing 3-D contouring or prismatic parts?

https://docs.plm.automation.siemens...id735964:id736004:cutting_stock_tolerance_opt

John Joyce
Manufacturing Engineer

NX 11 & 12.01 Vericut 8.0.3

If I asked people what they wanted, they would have said faster horses

- Henry Ford

 

[mechjames]

Hi John,
many thanks for the info. I am mainly making prismatic parts. How would this effect hole milling? Looking at the Gcode this is circular motion, G03 and G02 so not affected by intol/outtol values?
What are sensible number for small prismatic parts? intol 0, outtol 0.005 - is that ok?

thanks!
James

 

[joycejo]

For prismatic parts I would leave it at the default values.
and not change them. It will only slow down the processing time. If the tool path is a straight line, or circular moves it will be correct.

John Joyce
Manufacturing Engineer

NX 11 & 12.01 Vericut 8.0.3

If I asked people what they wanted, they would have said faster horses

- Henry Ford

 

[Tingsryd]

Some time ago GTAC mentioned or Siemens published that NX will output exact offset calculations with the exception of using the tolerances on everything else, such as a Z-level profile operation cutting a tilted cylindrical face, such as a blend on adjacent faces which have draft.

I'm not sure about helical milling a cylindrical hole and then not outputting G02/G03 moves with Z's. You are then posting linear G01 moves and I don't if the linearzation is happening in the operation or when posting.

As for model tolerances they can affect tool path accuracy. A while back I had a fixed axis 3D area milling path that was not quite cutting as accurate as I would have liked and GTAC tracked it down to the modeling tolerance. Not sure if this is still true but it's something to keep in mind when 3D contouring as John mentioned.


On a tangent...
We used to be bothered by the North American Cam Tool rep whenever he passed through town and he'd ALWAYS try to put down every other cam system. Their company position on tolerances is they are the ONLY software that performs exact offset calculations and everyone else is using faceting. While it is a partially true statement in reality Cam Tool has to interpolate some moves using tolerances such as the situation I described previously. However to this day they state they are the only company that exactly offsets tool paths which is an outright wrong statement. I think they also started using something similar to NX cut areas and they also claimed that was unique to Cam Tool!

NX 12.0.2
Testing 1899
EVP's

 

[mechjames]

Hi Tingsryd,
many thanks for the info. Very interesting. All good stuff to know...

cheers, James

 

[Dawson70]

Another item related to tolerances is in fixed contour/surface area. The default for cut step when you edit the drive method is Number: first cut 10 & last cut 10. I've attached a very simple file that shows how this default can scrap parts. The bad part is that it's hidden by default under the more tab which can make it easy to forget. Zoom in on the corner by x-y zero and replay them both to see what I'm talking about. Changing this to Tolerance: intol .001 & outol .001 fixes the problem. I've submitted an IR about this years ago and even had a conference call and they will not change it or put it in the customer defaults. Just a friendly heads-up if find yourself using this method.

 

[Tingsryd]

@Dawson70
That's a great example to be careful of! When using Number cut step setting I noticed the cut step-max step setting will affect that scenario as well and will clean it up a bit but still seem very archaic and something to avoid. Personally for fixed axis machining I use Area Milling and Flowcut about 99% of the time and thankfully those operations do not use the number setting. I can't imagine why it is still used other than perhaps as a legacy operation for a relatively few, large customers who have a lot of influence on Siemens.

NX 12.0.2
Testing 1899
EVP's