Organize the CAM Process

[ionelz]

01. You put the Stock on Wise

02. Machine the Part (TOP Machining)

03. Put the part 180 deg in Wise for Bottom Machining

How many files you have for a Manufacturing Part ?

I mean, do you have one file for TOP machining and another for Bottom Machining

What is the best way to organize the process ?

[Stefan_Pendl]

The best way is to have each setup in its own part file. This makes it much easier to do machine simulation of each situation.

If I remember correctly the machining line planer, included since NX 10 at least, should simplify the process of creating multiple setups. There is a video by @TomvantErve in the community.

[jkane1]

We do recommend that users make a new file for every machine setup they create. This has a few advantages.

1. File managment. Other users opening your file will always know what side is being machined for the single setup.
2. Smaller file sizes. Each setup file has only the operations and tool path data for that file. This means better perfomance.
3. Design protection. A proper manufaturing setup file brings the designed part file in as an assembly. This means that the CAM programmer cannot modify the original part while creating tool paths. He can create a copy of the geometry so that he can modify it for optimal tool path creation, but the original design intent is protected.

On the other hand, all setups and tool path data can be made in just one file. Mutiple MCS objects can be made for each setup on the part. The operations under each MCS in the Geometry View will be oriented to their parent MCS. This has the obvious advantage of having to manage only one NX part file rather than several files together.

The choice is up to you. Siemens has what we consider to be best practices, but your workflow should dictate what is right for your shop.

[ionelz]

Thanks all. I am in practice mode ! I am doing this :

- Create TOP file asm : add Part - add wise/clamps - link body all

- Create operation for TOP machining

Now I have a problem.

- When create Bottom file, I want the IPW from Top and I can not bring it to file (NX 11)

- But if I create parasolid of IPW (which I do not want), I have another problem since wise setup from Top it is not good for Bottom !!!

Also, is anywere a Setup in NX to put a clearacnce to "Specify Check". I see the Tool is JUST avoiding it but I would like to put like 1mm clearance to it.

[ionelz]

Hmmm, I have Manufacturing but I do not have File - New - Manufacturing option ! 

This is maybe the reason for IPW

[jkane1]

Edit the Workpiece object in the second setup file. Select the same part geometry as before. Now in the Blank Geometry definition, select the pull-down menu at the top and select IPW - In Process Workpiece.

Now select the Select Source for IPW button and browse for your first setup file. Select the Workpiece object from that file and select OK. Select the Update Local IPW from Source button and you should see a facet model in the graphics. Select OK and the roughing operations will use this to calculate IPW regions.

Let us know if this works.

[ionelz]

"The part containing the source for IPW must reference the same component for Part geometry as the work part"

[Stefan_Pendl]

That is not a problem:

First setup:

CAM-Part-Machine-Top
    |
    +- CAD-Part

Second setup:

CAM-Part-Machine-Bottom
    |
    +- CAD-Part

You always have the same CAD-part file as the component in each CAM setup part. The fixture, machine, etc. can be different, only the design part must be the same.

[ionelz]

Got it, thanks a lot...

[JSchraitle]

Dear jkane1,

I hope one day Siemens wakes up an notices their recommendation is against FBMs principle to do generate all machining operations in a single CAM part.