NX CAM / Mean Models...

[Shadowspawn]

Question of the day.... Is it possible to CAM program to the "mean" (think even split) of the tolerance value of a surface? ...for example, given a surface height of 1.000 inch and a tolerance value of +.030/-.000, can you program CAM to cut the surface at 1.015? ...and can this idea be extrapolated to a non-planer free form surface?

TIA

Regards,
SS

CAD should pay for itself, shouldn't it?

 

[Jaydenn]

You can add or subtract "stock" to any toolpath. It's a manual adjustment you make.

Is this what you are refering too?

Jay

NX 6.0.5.3

 

[Shadowspawn]

To be honest, I'm not sure....
Our lead CAM guy wants the CAD group to remodel all of the customer models to the "mean" of the tolerance value to facilitate his programming... I contend that it's a bullshit request, he contends that it would speed up the programming and make the CAM group more productive if they don't have to do the CAD guy's work....blah, blah, blah, ad nauseum. Yes, there's alot of bullsit politics involved and it's basically a pissing contest, but since I'm no CAM programmer, I can't really say with certainty what really is best for the company. Thus the original question and btw if it makes any difference, these are not exactly simple parts to model (think turbine blades).
Any insight would be appreciated...

Regards,
SS

CAD should pay for itself, shouldn't it?

 

[looslib]

The CAM guys can add stock on a toolpath or use a tool offset to leave a certain amount of stock. Machining stock for a finish pass can be added to the surfaces when defining the tool paths. Instead of it being finish stock, it becomes the finish dimension if they want the pat to mean size. It does ass some work to the NC Programmer's load, but it has to be done someplace.

Building the CAD model to nominal/mean size has always been an issue. The model should always reflect design intent, which I have always inferred to be nominal size.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[jerry1423]

When I am asked to create the model to the mean I include both dimension values in the expression:
p100=(1.030+1.000)/2

 

[John2025]

Not what you want to hear, but we always try to model to the mean. I think it falls under designing for manufacturability. That's a designer's responsibility, IMHO.

 

[Tingsryd]

I agree with John2025. Ideally the model should be what the cnc programmer is going to apply tool paths to. As it turns out it can often be more complicated than that. For example some questions you have to ask yourself might be: how stringent is your design and programming process? What is the preferred method? Do you need to xfer data back to your customer or another 3rd party?

From a designer point of view, moving faces around, especially non-prismatic structures can be time consuming to say the least or downright nearly impossible if you are working with non-parametric spline surfaces that may not easily change, such as simplifying faces, re-blending and offsetting faces.

From a programmer point of view, well, it can be the same as designer. Some programming situations are easier to deal with than others. You might want to speak with them and get a bit finer grained with your discussion. For instance if your programmer needs to use a Z-level profile operation, which is 2.5-D, it works great if you specify the same amount of stock on floors and walls. Not so great if the floor and wall stock is different and they are anything other than straight walls and flat floors. It can be even worse if there are large angles involved, without the programmer being capable of predicting the end result. This is because that type of operation is not suited for that application. On the other hand if a 3-D contouring operation can be used then there is much more accurate control over the result. It all depends on what the programmer can/cannot do and what the designers can/cannot do. Being informed about both processes and having open minded people is key here. The burden might fall on programmers sometimes but on the designers other times.

You mentioned you are not CAM savvy (sugar coated!) so I recommend listening to the programmers and designers then try to make the most informed decision possible.



NX 7.5

 

[DaSalo]

I think the bottom line has to be that you model what you want and then the CAM programmers do what they need to from there. With conventional machining this is very straight forward but when you get into EDM and other unconventional techniques this is not at all straight forward. For EDM programming you are always rebuilding surfaces, offsetting, etc. to account for overburn, recast layers, etc. There is no way that the designers could ever take all of the variables into account. In your situation, where you have customer geometry, you really have no control over any of this. The only question is which team has the better skills and resources to get the work done most efficiently. If your CAM guys don't really know their way around a model and only know how to drop simple toolpaths onto existing surfaces then perhaps you will be better off having the CAD team deal with it. If your CAM guys have solid CAD skills then there really shouldn't be any issue; they would just crate what they need and be done with it. Perhaps this is more of a training issue than anything else.

NX 7.5.5.4 mp01, NX 8.0.1.5
Tecnomatix Quality 8.0.1.3
PC-DMIS 2011 MR1