Drawing view to lock to one parameter option

[claire.ogilvie]

Hi

I have a parametric assembly of three parts. The parameters allow us to update the model based on the flange size the assembly is required to be attached to. 

I would like to have one drawing that covers the range of models we have set in the parameters and have a set drawing view for one size (DN600) so that when the model is updated to a larger size say DN1000 the drawing and dimensions still stay at a DN600. Our dimensions will be A,B,C with a table of dimensions for corresponding flange sizes.

I cannot seem to get a View Representation to lock to a specific parameter view. 

Any suggestions would be appreciated. Beyond this specific example I would like to know ways to get idw's to be more dynamic. We have many ways to automate and speed up modelling but we need better ways of updating our drawings to truly streamline our processes.

Thanks!

[SharkDesign]

Are you saying that no matter which part you put in the drawing, you want them all to take up the same amount of paper?

You could try auto scaling them with iLogic, various resources here:

https://forums.autodesk.com/t5/inventor-forum/ilogic-and-scaling-view-size-automatically/td-p/700314...

[claire.ogilvie]

@SharkDesign  I guess I am asking for that. That would be a very nice solution for some of our products.

Ideally for this particular solution I want just one static 'standard' drawing for all parametric sizes but I need the model that changes in size to be linked to the standard drawing that doesn't change.

[SharkDesign]

I don't quite understand.

 just one static 'standard' drawing for all parametric sizes 

Do you mean, you have part a,b,c and drawing a,b,c. The drawings B & C look the same as drawing A except dimensions are different?

What does this sentence mean?

I need the model that changes in size to be linked to the standard drawing that doesn't change.

[claire.ogilvie]

the attached image is the example of the drawing that one of our manufacturer prefers with the dimensions taken from the table according to the DN size requested.

[johnsonshiue]

Hi Claire,

I think this can be done fairly easily using Model States or iPart/iAssembly. Essentially, you just need to show the drawing views of one variation. The rests are captured on a table.

General Table in the drawing can retrieve the table data from Model States, iPart/iAssembly.

Many thanks!

[claire.ogilvie]

Hi @johnsonshiue yes this is what I thought I should be able to do.

Would my issue be that the model is parameters and not iAssembly? I cannot seem to assign a specific parameter option to a view, the view always changes to the current model status.

Thanks!

[claire.ogilvie]

Hi again @johnsonshiue I just researched 'model states' briefly and this is only something for Inventor 2022?

Thank you

[A.Acheson]

Model states are only inventor 2022. Outside of model states, views control only visibility of parts but not size. The individual files controls the size of a part/assembly. It sounds like your at a crossroads in design. There are a few ways to move forward but I would suggest research each method to ensure you understand the disadvantages and advantages. 

Have you used iParts to create the part that changes in size? An iAssembly will be a defined assembly utilizing iParts or standard parts but does not use custom parameter of parts/ iParts (i.e will not allow on the fly changes in length as an example) They effectively layout out the file naming in advance and allow parameters be assigned to these individual files. The individual files are called members and these are all controlled in the factory file through an excel style table. Each member created from the factory is actually a derived file linked back to the factory it was created from. So any changes needed will require opening the factory and pushing the change out to the derived file/member. 

You could also simply change parameters and save files as unique set either manually or if you wanted a semi automated configuration using ilogic. Both of these have the drawback of no central factory file so perhaps more difficult to see the linkages and no way to create tables easily for parts lists