I need to mill a chamfered pocket, as seen in the first picture. I use a 5-Axis contour profile operation to get the toolpath. The intol and outtol are set to 0.001mm.
Using an external NC simulation, the operation results in shape deviations of about 0.01mm:
Also, the IPW analyzer shows deviations of the same magnitude:
Is there a way decrease the deviations? I have already adjusted the chamfer and distance tolerance, but that had no effects.
I am using NX 220.127.116.11 by the way.
Lowering the cutting step had no effect.
I have also created the chamfer as a revolved surface to make sure, it is a ruled surface, but still the same:
Switching between Line and Arc has also no effect.
No difference of adjustments of Intol and Outtol between 0.0001 and 0.005.
I suppose that cut step or path tolerance has to always check the part surface and not to collide with it.
Isnt it about ipw resolution?
interesting topic :-)
I created a part with two geometries in it. One is where you build the chamfer with the chamfer option and one where you actually "design" it.
Two Contour Profile operations are done and I can get an accuracy of +/-0.0005 with a 0.001 outtol/Intol in the operations (just a few with 0.001). In both designed geometries!
So let me try to explain to you what might cause the bigger tolerance in your cases. In CAD you do have the possibility to define the tolerance that your design element should have:
So if you'd like to have an accuracy of 0.001 in CAM, it does not make sense to model a chamfer with the default setting of 0.01. So if the CAD part is dessigned with a "rough" tolerance, then the surfaces and vectors are not accurate enough for the toolpath calculation.
A little CAD background. A modelling tolerance of 0.1 doesn't mean, that the modelled body is 0.1 smaller/ bigger. The tolerance is calculated into the Tolerance Modelling. Thus transitions from surfaces (when is a gap really an opening) and also the vectors, at which the Contour Profile is calculating the tool against.
But I highly doubt, that the machine tool can really be as accurate as it is in NX CAD/ CAM. 0.001 is a tough goal :-)
If there are any further questions, please let me know.
thank you for your detailed answer! I already tried different design tolerances of the chamfer, but couldn't see any difference.
Of course I don't expect the machined part to within +-0,001mm, but if the CAM Systems induces 15µm deviation, I won't get anywhere near my goal.
I would be highly grateful if you could have a look at my file to be sure, that the settings are not messed up. By the way, did you alter your modelling preferences?
I tried to program you and tweak some parameters to get you a better result.
I changed the tolerances in the Extrudes to 0.001
Set the Max Step value to 0.001
But what made the most change was useing the smooth connections in the NCM dialogue (please look at the parameters):
I didn't do any changes to the Modelling defaults.
Used NX 18.104.22.168 for this.
Would be nice if you can have a look at the attached parts and let me know if it does address your needs :-)
when I open the file yout attached and chose Analyze IPW with automatic Min/Max limits,
I get the following result:
So, still deviations between -0.005 to 0.007.
However, I could achieve tolerance below 0.0005(!) when using an offset curve of the contour as drive method.