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How to hide features in assemblies?

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Re: How to hide features in assemblies?

It seems that having separate assemblies represents the work flow most realistically in this case, but keep in mind that if you want to have the pre-machined and machined versions covered in a single drawing, you can always add both models to a single drawing.

Re: How to hide features in assemblies?

Yes for most of our clients we do exactly that, make seperate welding and machining models and drawings, but this one specific client has different SOPs than the rest, so have to follow it. 

Re: How to hide features in assemblies?

Why PTC is not including this functionality in Assembly level, this can avoid generating two different models and mismatching data error.

Example:

Case 1: here, if we have a design change request after releasing, will have to revise both models and chances missing to update Assembly 1, if the change applicable with Assembly 2 (model) level or vise-versa.

 

Two different model (Case 1)
Assembly 1   Assembly 2
part 1   part 1
part 2   part 2
part 3   part 3
part 4   part 4
part 5   part 5
part 6   part 6
part 7   part 7
part 8   part 8
part 9   part 9
Extrude cut1   Extrude cut1
Extrude cut2   Extrude cut2

 

Case 2: here , if we have change request will have to update one models and no chances missing to update 1st level (i.e., Assembly 1 stage) if the change applicable with 2nd level (i.e., Assembly 2 stage) or vise-versa.

  Assembly 1 - single model (Case 2)  

 simp rep

status

Simplified rep 1   Simplified rep 2  simp rep status
  part 1   part 1  
  part 2   part 2 Exclude
  part 3   part 3  
  part 4   part 4  
  part 5   part 5 Exclude
  part 6   part 6  
  part 7   part 7  
  part 8   part 8  
  part 9   part 9 Exclude
Exclude Extrude cut1   Extrude cut1  
Exclude Extrude cut2   Extrude cut2  

 

 

 

 

Re: How to hide features in assemblies?

You can merge the welded parts together into a single prt. file. In this part, you can do the machining as well as make a simp rep, since it's a part file.

 

You will find the merge function on: Model tab > component > component operations > Bolean Operation

 

NB! You will need to make a (empty) part file first and assemble it in the main assembly, so that all the assembly parts can be merged into the new empty part file wich you will be using from now on.

 

Re: How to hide features in assemblies?

Not sure if that helps any, but just wanted to add that you can make your assembly level cut visible as a feature in the sub-component part being cut (see the "Intersect" tab in the definition of the assembly level extrude feature).

Then in that part, you can define a simplified rep which has the cut feature excluded...