Inventor | Some Quick Tips From A New Design

I began a new machine configuration recently, and during the process, picked out a few tidbits that I thought some of you might like. Many of these are from older workflows, and some are new to 2012..

Frame Generator Considerations

If you are new to Frame Generator, you may have run into problems with frame alignment on 2D Sketch Geometry. Picking frame locations to be applied in a single pass causes numerous frames to offset to the wrong side of the profile. Some good, and some bad. To make matters worse, there is no way to individually alter these while applying them as a group. There is a better way – it is all in how you apply the frames.

You cannot set all frame members in one shot.

If all the planets are not in alignment, at least one frame member will be wrong. You need to set them in planned stages.

In the example below, you see how the Inventor’s Frame Generator defaults to the center of the frame. No problem, we just pick the correct alignment. Now we can pick the remaining frame locations IN-LINE, and Inventor will align the remaining frame members accordingly. Then we can move on to the next grouping. Repeat the process of getting the first in a run set how you like it, and Inventor will apply the remainder properly.

Grab multiple frame members to be trimmed along same plane

Now that the frame is placed, I need to trim off the lower section of excess frame. I spoke of the Trim to Face tool recently, that is a great way to hack off frame members when the underlying sketch geometry needs to be long.

New users may not have figured out that you can select as many frame members to trim as you like, all in one command instance. The button in the dialog says Pick Frame Member, not Members, and many similar functions only work with one selection.

In this case, you can pick as many as you need to. Once you have them selected, just pick the Face button, and select any face in the assembly. After you hit apply, each frame member will be hacked off at the plane of the face indicated. One thing to remember is that this command will cut the smaller end off, and leave the longer one.

Make Part

This and it’s sister ‘Make Components’ are just brilliant. I was all ready to send my frame to a weldment when I realized I needed some modifications. I added a plane and sketch to my skeleton, but in order to get from the sketch to a part in the assembly, you will still have to:

Create a new part file
Derive the sketch from the skeleton part
Save it
Open the intended target assembly
Place the new part file, and ground it.What if I told you it can be done in one step? It’s bad ass.

Pick ‘Make Part’ from the Manage Tab’s Layout Panel. A dialog will appear, allowing you to select your geometries and features, name both the part file, and the target assembly file, as well as selecting BOM structures and templates too.

Inventor creates everything, and will package it up in a new Assembly, or insert it properly into an existing one.

2 Serious Time Savers

Now it’s no problem to open that part file, and develop the part as needed. A quick pull and this mounting plate is started.

Notice I used the in-line Parameter naming functionality. If you use a lot of Parameters like I do, this will cut down on the all too frequent trips to the Parameter table.

When done I gestured the close, rather than picking it from the mini-toolbars. This functionality lets us bypass the marking menu, and still use it’s functions, even though we can’t see them. Just right-click in the Graphics View Area, pull to the right, and release. After a while, you’ll memorize what’s on the marking menus, and will get the motion down to a flick of the wrist. This is especially cool when you are using in-line commands that feed on one another.

During my Publisher class at AU 2010, I demonstrated gesturing daisy-chained commands without deselecting the sub-assembly. Using Gesturing, I completed 5 or 6 commands, including explodes and Sub-assembly moves with and without trails in less than 15 seconds. Gesturing rocks! It just takes practice.

View Representations in Parts

I re-arranged my components to organize my frame welding better. When I replaced the necessary Subassemblies, it was a mess with extraneous model features sticking out from the rear shield component.

Easy fix. Inventor 2012 now provides View Representations to Part files. Once saved in the part file, these View Representations, like in Sub-assembly components, are accessible through the expanded component tree in the Assembly Browser. I had previously established my Part View Representations, so now all I have to do is select that representation from the component in the Browser.

For Part Components, select ‘View’ in the component tree, and pick ‘Representations’ from it’s context menu.
For Sub-Assembly Components, Select ‘Representations’ in the component tree, and pick ‘Representations’ from it’s context menu. There the respective views for each type can be changed easily.

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Inventor | Some Quick Tips From A New Project