Assembly Modeling - CREO PARAMETRIC

[AC_4632076]

Hi all, 

I was looking at getting some guidance with simple assembly within CREO. 

I've been tasked to a create an assembly in which I am given 2 complete parts as well as am required to create a third part for this assembly. 

When creating the third part of the assembly  is should be drawn that A1 = B1 and A2 = B2, meaning that this component updates automatically depending on the modification made to the first two components which exist in the assembly. 

How do I go about this? Do I create a seperate brand new model and then add this to the main assembly. OR should I assemble the first two parts together and then create a new part within this assembly.

This is to made made that no clashes or gaps happen within the main assembly model 

[tbraxton]

There are multiple ways to do this. You can work on the new part in assembly mode or in part mode. You also can use a multibody part design if you are in Creo 7 or higher. I would build part B as a new part in part mode and use one the following methods. You can build the new part in assembly mode, but I would not pursue that in your case as it has much more opportunity to create unwanted references.

These are two strategies but there are other ways to do it as well.

One option is to write the relations controlling the parts in assembly mode. In this structure part B dimensions drive part A. To do this build the assembly with all required parts. You can then write relations in part A that will use the values of the dims from part B directly. You will need to use the syntax including the session ID of the parts when writing relations. See this link for details on this: About Entering Relations in Assembly (ptc.com)

Another option: Note this technique is not likely taught in your curriculum. In this structure the Notebook file drives parts A & B directly.

I would suggest that you create a new part in part mode and use relations to drive the dimensions controlling the interface geometry. You can easily control the dimensions using a notebook file. About Notebooks (ptc.com)

In the notebook you will create parameters for dimensions B1 and B2. You will then declare the notebook to each part. Once declared you can use the values of B1 and B2 from the notebook in the part model relations. You then write relations in each part that use the B1 & B2 values to control the features in each model. When you need to update the model you can just change the values of B1 and B2 in the notebook file and regenerate the assembly and all parts will update.

[BenLoosli]

Are you a student taking a class in parametric modeling?

[KenFarley]

Hmmm, what clues led you to that question?

[RPN]

Yes layout/notebook is an option, but than you have to change the value in the layout and this was not requested. 

Here an other way to archive your goal:

• You have all 3 Model created and assembled 
• Change the model tree to display the session ID for each component 
• Assume that component B has Session ID 25 and the symbol name D20 is equal to B1
• Pick on component A and the dimension corresponding to A1
• Enter D20:25
• Answer yes on ask to save the relation

Done,

Now the dimension in component B drives the one in A as requested. 

Getting extra points: 😎

With an additional relation you may add the model name of ID 25, because you will forget  „Which one is 25“ 😉 like model25name=PTC_COMMON_NAME:25

Or if needed add your own parameter in source to  display the name and link it into the target. 

Good Luck