Error of part having features defined in context of another assembly

[Spurs]

In the past I have used the a procedure that I will describe to sucessfuly to create a workpiece model by simulating what happens during machining of the workpiece. I need to change this approach due to the complexity of this new project I am working on. This new complexity is causing me a problem and I am looking for advice.

What has worked in the past is the following:

I created a model of a Tool - lets call it "A0" - A meaning the tool and 0 meaning positioning of the tool in 3D space in the model.

I then created 2 other versions of Tool A in 2 different positions in 3D space - all models are named A1 thru A2.

Next I create a simple workpiece part B.

I then create an assembly of all the parts A1, A2 and part B
Since they are all in the same co-ordinate system, all I need to do is line up the origins of all of these different parts in the assembly and they are in correct position.

Then using the cavity feature individually between each tool A1 and part B and A2 and part B, the form of part B is "machined" into its final model shape.

This works fine.

There is a new twist to this new project.

The positiong of models A1-A2 is now much more complex. I really dont want to spend days coming up with the new complex positions.

It is easier to divide the problem to 2 simple positions of tool A, plus 2 manipulaitons of the positons of part B.

So this time i tried doing the following:
Create models A1 & A2 - same tool in 2 different positions.

I then create a simple workpiece B1.

Then I create assembly Assembly1 using A1 & B1 and do the cavity command.

Now I have a part B1 which has a cavity in it. I do a save as copy on B1 - naming the new copy B2.

Then I reopen B2 and move it to a new positon in the 3D space.

Then I created a new assembly Assembly2 using A2 and B2. Now when I do the cavity funciton I get the following error:


This part has features defined in the context of another assembly. You can edit the part, but cannot create any external references to the components of the current asselbmly.

The cavity funciton will not work.

What can I do to get around this problem. I really do need to manipulate both A2 and B2 into new positons prior to the cavity function.



I know that I cannot Create Assembly 1 and then manipulate part B inside assembly 1 cause this does not retain the original cavity positioning.

Anyone have any suggestions?

Thank you in advance

 

[Eltron]

You can always save it as a dumb solid or just break the references to the original assembly.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[dgowans]

Spurs,

If I read your post correctly, all you need to do is enable the following option:

"Allow multiple contexts for parts when editing in assembly"

This is found in your system options.

Obviously you will need to be mindful of all the external references so that you don't end up chasing your tail, but I believe this will accomplish what you need.

 

[MadMango]

Chasing your tail... the reason I would do as Eltron stated. It will require you to create a new B2 model if the B1 model ever changed, but there is less possibility of someone else messing up your model.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[drawoh]

Spurs,

You seem to be making this very complicated. When I design machined parts, I create the initial block, then I remove material. For each material removal, I try to understand how the shop will do it. I would not be trying to model the process unless I was the one programming the CNC mill.

JHG

 

[Spurs]

dgowans - changing the context option solved the problem - thank you for the advice.

drawoh - the approach I am using is the same approach as how the shop does it. They change the positioning of both the tooling and the workpiece on a continuous basis as they remove material. In fact, to simplfy my explanation, I only told you that there are 2 iterations - in actual fact, there are about 200 iterations. What I am trying to do is that by knowing the cutting tool, and by knowing the manipulation of the cutting tool and the workpiece, I am trying to predict what the final part will be.


Madmango - changing of the models is not an issue - i have created macros to do everything from start to finish so if I need a revision I just change the input function.

 

[Spurs]

Eltron

How do it turn it into a "dumb" solid, or break the references?

 

[Eltron]

File- Save as- iges, stp, or whatever your pleasure. As far as breaking the references go, there should be a place to list the references in the file menu where you can select to break them. I'm not at a 'puter with SW right now, so I'm not 100% sure where to send you.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[buyputs]

Spurs,

I had the same error message. You can break the references as Eltron has suggested by right-clicking a part, feature, sketch, etc. in the "FeatureManager design tree" and selecting "List External Refs." You can then "Break" the reference to completely remove it (if you only need it for the original part and the design won't change) or you can "Lock" the reference so that it will stop updating (this also makes the system more stable and less buggy in my experience).

Breaking the references will definitely get rid of the error message, but you may have to start over if you change something (a tool position, for example). I would try think Locking the references first and see if that works.