Inventor 2015: Easiest way to handle 6 configurations?

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So I’ve got to do drawings for my advisor using Inventor 2015. As is the case with any boss, they say X but sometimes want Y, so I want to know the easiest way to handle configurations and drawings. I have plenty of experience in the past, but considering I need to make manufacturing drawings I wanted to ask to see if there is a better way.

It’s model of a RHS frame with 2 different length options and 3 different attachments on the front. It’s a bit like a trailer with 3 different wheel and drawbar options for 6 options total so it will be done mostly in FRAME GENERATOR.

I would normally make 2 different length frames and 3 different other frames and make 1 assembly with 6 configurations and make individual drawings for all components and assemblies to minimise work.

Realistically, the description is a working generalisation and the problem becomes when my Advisor changes his mind and wants length option A to have a different width as well (making more then 6 combinations)… you start questioning whether you should have drawn 6 different CAD assemblies/models in the first place rather then use assembly configurations which get extremely messy quickly.

How does one handle this in modelling and drawing environments?

This sounds like a one sheet drawing.

Set up the views for one frame.
Add all the dimensions as usual.
Replace the dims with letter, e.g. change 14.25 to ‘A’.
Create a table on the sheet with corresponding dims for each letter.

Sometimes, if you have different measurements along one side, you can do something like, ‘A + 4.25’

I agree Joshmings, that works, particularly for the length change configurations.

The 3 options though in my experience usually are never as simple as the attachment on the front changing! The net result is you can’t consistently reuse a drawing of the higher level assembly with the options. Model configurations alone can get messy.

So to clear up my question, if you were using frame generator would you just change the length back and forth or just make two dimensions on the drawing and only show one model?

Generally, for build or inspection you need to capture both dimensions on the drawing. In that case, I would have two assy numbers with generic ‘A’ dim and a table that provides both.

You can keep the configurations on your model and only show one on your drawing. If the assembly is quite a bit complicated though, you may want to dimension out one assy config, then copy those views to another sheet and switch configs for that assembly.

How do you copy views? I only know of “SAVE AS” to another drawing and modifying from there.

A simple copy/paste operation, but I’ll refer you over to our pal John over at Design & Motion :smile:

Oh, so you just mean inside the same IDW. It doesn’t work across IDW’s from memory.

Right. I thought it worked across them too (will need to check.) But the other option for putting it on a new drawing, instead of a new sheet, is to save out a new drawing. If you’re using vault, you can use ‘Copy design’. If not, it takes some fancy save/rename work–Save parts/asm/idw into new folder, rename parts/asm, open drawing, when asked to find reference, select the renamed parts/asms.

  • Draw all 3 attachments in separate .ipts

  • Insert blocks of fittings into another .ipt to model length/config one.

  • Place fittings in a .iam and make componets on config one and place them in said .iam

  • Copy config one and make length changes.

  • Copy .iam and replace length parts w/ new make components from config two

  • Create .idw and populate sheets per needed.

  • Copy .idw and replace model references (manage tab/modify) in copied .idw w/ second .iam

Do the same for other views you need by copying master .ipt/ .iam