Modify Length of Vendor Supplied .stp file

[jcolacino]

Good Evening,

I'm very new to Inventor and have what I hope is a quick question.

I have a 3D .stp file for a product that ships in 6' lengths. We cut this to length when we use it and I was hoping I can easily modify just the length as I place instances of this item into an assembly.

I attached the file here for reference and looked for an easy way to do this at the time of placement but no luck. 

Any help would be great!

Jim

jcolacino@colacino.com

[Xun.Zhang]

Hi Jim,

Welcome to Inventor world!

I am not very clear about your question, Are you talking about to control the overall length with parameter input? do you want the U unit shape change accordingly with the length change ratio or you want the U shape always the same?

Any more details?

For this specific sheet metal part, it's very easy to be rebuild from scratch with Inventor sheet metal, I believe this is the way to full control it with parameter.

Please refer to enclosed file and the U unit length is 1 in, you can control the pattern number to control the overall length, for example, if you pattern occurrence is 100 ul, then, the total length is 100 in.

In addition, you can also leverage iPart to create different length members if you want.

Hope it helps!

[jhackney1972 · Accepted solution]

After opening the STEP file you will have a base component of 72 inches.  This measurement is not in the file at this point.  Take a look at the screencast and you will see a method of cutting this to any length you desire.  The nice thing about this method is the distance of the new work plane is the new length of the part so you can use the variable directly to your parts list if desired to report the length.

You will of course be saving each part by a new name as you make them.

[Mark.Lancaster]

@jcolacino

Adding to the posting

Files that are exported from other CAD applications are imported into Inventor as a "dumb solid".  There's no feature history and no parametric information.

One more side topic..  I know its only an email address but you shouldn't share personal information here such as an email address for security reasons.

[mcgyvr]

In addition to the solution posted by jhackney above you can also just cut away the parts you don't need with an "extrude (cut option)"

That could simply be a rectangular sketch that just chops off what you don't want or project the end profile and extrude (cut) 5ft off it or whatever..

[Anonymous]

This looks great and I'll try it as soon as I get back to the office. You guys are all fantastic

[kelly.young]

Hello @jcolacino the previous replies will be the easiest way to work with this .stp to trim the size quickly.

It would also be easy to just re-model from scratch. See attached.

You can drive the length of the pattern depending on how long. 

Not sure what the end game is but I always find reverse modeling suppliers parts and converting to parametric models helps in the long run. 

Another idea to think about, depending on the complexity of your part, you can use the Feature Recognition add-in to auto-generate known Inventor features. 

App Store: Feature Recognition

I ran it on your part over lunch and it took quite a while due to the repetitive cuts but was successful. See attached.

For simpler parts it might be helpful, but in this situation it was a pretty terrible idea. Not really meant for patterns and came in with 71 Work Planes, 144 Chamfers, and 201 Extrusions, which isn't useful. I just wanted to see if it would work and what it would come up with.

Created in 2018 without asking your version so hope you can open them. Nice Hoover Dam pic, love that place!

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