Showing results for 
Search instead for 
Did you mean: 

CAM collusion toleranced hole

Valued Contributor
Valued Contributor



I would like to know is there is a way to adjust the Diamter of Holes with PMI tolerences. 


- for example: I have a hole Diameter 20 with tolerances +0.2 and +0.0 

The middle toleranced hole would be 20.


- Problem: when i create the model the hole is 20 and when i make a CAM-Simulation

with a tooldiamter 20.1 there is a collusion.


Is there a solution for simulating a toleranced hole where the diamter ist smaller then the 

tool diameter without a collusion ? 


Re: CAM collusion toleranced hole

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

1) Always use symmetrical tolerances.  I know engineering won't want to hear it, but that's (pretty much) what you will actually do in manufacturing...So either they do it that way to begin with, or mfg will do it anyhow (see #2).

2) Create a "manufacturing model" part (assembly of engineering part w/ linked solid).  Modify (typically using synchronous methods) all the non-symmetrically toleranced faces to the middle of the tolerance band.  (you can also add fillets/rounds/chamfers that engr left off, add grind stock, etc.)

What would be nice is if mfg could "charge back" the cost of the mfg model creation to engineering - so engineering sees the true cost of doing it they way they want :-) 

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled

Re: CAM collusion toleranced hole

Siemens Phenom Siemens Phenom
Siemens Phenom

You can use a WAVE body and synchronous technology - Resize Face to change the diameter of the hole ... but that's not really needed.


Just use the new hole making operations. These allows you to select tools with a diameter larger than the hole (initially, you will get an Alert saying: Tool Diameter is greater than Feature Diameter. Tool will gouge the part but that's exactly what you want in this situation).


The tool path will be generated just fine, even if you have "Gouge Checking" active. The software assumes that you made a contious decision to use a larger tool and doesn't report this as a Gouge.


MB3 Tool Path -> Gouge Check will NOT report this as a gouge either. The same is true for Gouge checking in Verify and Simulate.


We call this "Allowed Gouges". This isn't only important when you drill using a larger tool, it will also come in handy when you machine chamfers that are not modeled or tap holes (where the nomial diameter of the hole is typically set to the "thread_tapped_drill_size" diameter (e.g. 5.2 mm) which is almost always smaller than the "thread_major_diameter" (M6).


On the topic of terminology: NX differentiates between gouges (ie. damage to the part while cutting in feed rate) and collisions (rapid the tool into the part).


NX CAM Development

Tom van 't Erve


Learn online

Solution Information