Very new to inventor 2012 coming form solid edge way back in the day (1998 to 2008) to autocad 2d. getting ready to move to the inventor and trying to figure out some things. searched videos , training etc but not even sure what to call it. but my questions are this. (if you can link a triaing or you tube video that would be great).
My questions are this
1. I design stamping dies and I will want to build sections from a stock strip with the outside then adding hole, dowels etc. what is the best work flow for this? It is kinda the middle between top down and bottom up.
2. what is the best work flow for adding counter bore , dowel in the block and then having this tied to the mating block so if I move the location of the holes in the block then move as well?
Thanks in advance
Solved! Go to Solution.
You may find modeelling in a multi-body 'Master Part' helpful.
I put together some tutorials on the various meathods of modelling assemblies with Autodesk Inventor here:
(It says 'for woodworkers, but don't worry - the technique is the same, it's the subject that varies).
You might also look into Derived Components techniques.
Attach example problem here if possible.
Thanks for the link and good info. I have figured out a few more things. However , what I was trying to ask is to simply it let me give another example. Say I have a block with a counter bore. I create an assembly and add another block that is contrained using the orgin plans.I want to put a tapped hole in the new block where the location of the counter bore is in the other block. I figure out how to do this with a project tab and used a point but I can't seem to figure out how to link them so that if I move teh counter bore the tap hole moves with it.
Multi-body technique would be my preference for this example, but you might also search on 'Adaptive' in the help files. In your example, edit the second block in the assembly (Edit instead of Open), then start a sketch for the tapped hole center. Instead of dimensioning a center point in your sketch, use the Project Geometry tool and pick the counterbore diameter from the first block. Change the center point of the projected diameter to a center mark, exit your sketch and create the tapped hole. You will notice that you get a red & blue circular arrows icon next to the hole feature and sketch in your browser, indicating that the feature is adaptive.
Now when you exit the part-editing environment (i.e. return to the assembly), you will see the same adaptive icon next to the second box, and when you change the hole location in your first box and update the assembly, the tapped hole will move.
For holes, you could also use the Bolted Connection generator, which will do something similar, but more automated.
Option #1 - Make the whole thing a multibody part. Put the hole in the part file, and derive the part out into an assembly.
Option#2 - Use adaptivity in the assembly (Not recommended!)
Option#3 - Make the hole at the assembly level (Check out weldments for some nifty workflows)
Option#4 - Use the bolted connection generator (My preference)
I hope that this list gives you somethign to tihink about! Get back to me if you have any specific questions about your chosen workflow.
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