Instances

[jay.czerwinski]

Noob Here - Spent days trying to solve this via research.  Thank you for your help.  My Background is in Pro\E and Solidworks, and I'm trying to wrap my head around the methodology of Fusion 360 used at my new workplace.  

I have an extrusion with a specific profile.   I want to use different lengths of it in an assembly.  I want to be able to go to one place to update the profile/cross section, and all of my cut down pieces are updated automatically, as well as the assembly adjusting a little for the change in dimension of the extrusions' profile.  

Perhaps even - Inventor is where I should be trying this?

[TrippyLighting · Accepted solution]

Post a practical "real" example and I might be able to show you a workflow.

This is indeed much easier to do in SolidWorks or Inventor because both have their own versions of frame generators, that can make really short work of it. 

In essence you would create a sketch for your profile in a separate design.
Then you'd derive that sketch into your new design and use it there multiple times to create your profile extrusions.

To update the profile, you'd edit the design with the profile sketch.

While you can create multiple sketches in a single file and derive each sketch individually into other designs, I would resist the temptation to build a library with too many sketches in one file.

When you update only one of the sketches in the file, all designs that you used any of the sketches in will be out-of-date. Not just the one that uses the sketch you actually edited. 

[jeff_strater]

Good point, @TrippyLighting - I didn't even think of this as a frame generator problem.  I saw this as a configurations problem.  "Configurations" are a way to have a single template design, and generate different variations from that single design, using a table to drive the variations.  This project is currently underway in Fusion, but is not yet available.

For this specific workflow, there is a way to do that that is a bit awkward, but does work currently.  Put your profile by itself into one design (just the sketch), and then Derive that sketch into different components, one for each length that you want to have, or for each usage (e.g. "top horizontal rail"), which could be edited if the length changes.

[laughingcreek]

both frame generator and configurations would be welcome additions to fusion.

when I do need to reuse a profile, I put it in a component at the beginning of the time line (so it's easy to find for edits), then put copies of it in each component as a sub component, and use it to extrude. (one of the few times I will have a body at the assembly level).

attached is an example model-

[TrippyLighting]

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@jeff_strater wrote:

Good point, @TrippyLighting - I didn't even think of this as a frame generator problem.  I saw this as a configurations problem. 

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I've used configurations for this in SW, but in retrospect, because the only change was the length, that wasn't overly efficient. 

Aside from having an actual frame generator, I find the derive-sketch method quite efficient and lean.

For most of the stuff I do I don't even derive the sketch, because we use a lot of purchased AL extrusions where I work. I copy-paste/new the component with the sketch and then edit the existing extrusion to match the new conditions

[jay.czerwinski]

Thanks @TrippyLighting and @jeff_strater for the fast replies.   Please forgive me, but my new company job may feel my cross section and the assembly is confidential at this point.  I don't have a sample I can share immediately.    I think I understand your suggestions.  My initial thought was that F360 wants everything to be in one file.  But if I understand you right, I would make a profile section in a part, and then bring it in as an early feature for other parts to build, and then to an assembly.  

If I were to create a sample to post, I'd just do a hollow square tube 12' long.  Then I would make lengths of the tube into a picture frame for an example assembly.   After the assembly is done, the customer might want to see more of a rectangle than a square tube, or a plus shape instead of a hollow square.   I just want to go back and modify the cross section of the stock bar length, and have all of the post processes update.     In the sense of an instance, I look at it as being like a bolt with a logo on top.  I want to model one format that has a hex with a logo and threads below.  I would use a number of different size bolts and lengths in an assembly.  And after the matrix is done of all the variations, I may want to change the logo and have all of the bolts update, and in all of the assemblies they are used in.  

I will work on your suggested solution of saving out a separate part of bar stock first and explore that.   I've got to believe this is a common issue with users and I am open to a specific video if someone knows of one that correlates to the objective.    Thank you again and I will post my results - hopefully sooner than later!  😉

[TrippyLighting]

Here is a link to an example I created.

After clicking on download you need to provide an email address. When the download is ready you'll receive an email with a download link. Then you'll download a.f3xz file. That file include the frame and the file with the sketch for the profile.  

[jay.czerwinski]

@TrippyLighting 

Thank you for the direction and for the sample assembly!   As a newbie, the word "Derive" proved to be an important command in F360 = Insert>>Insert Derive.  I will watch for more videos on Derive.

This was my solution, but I was pretty slow at things -

1. Once I bring the sketch in from a different saved file, it is tricky placing it with a second operation to where I want to push/pull from.   I'll work on my training on Assemble>>Joint operations for best practices.  Seems that little origin hash marks are key. ?

2. Once the sketch is brought in to a New Component of the master component, it seems to always have a pencil next to it.   Although the stand alone file has a red lock (meaning good strangely enough), the imported sketch has a pencil - same with the sample assembly you provided.   The obsessive-compulsive in me wants to get red locks in all of the sub-component sketches, but I guess it is OK to leave as a pencil here?

Thank you again!

[TrippyLighting]

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@jay.czerwinski wrote:

@TrippyLighting 

2. Once the sketch is brought in to a New Component of the master component, it seems to always have a pencil next to it.   Although the stand alone file has a red lock (meaning good strangely enough), the imported sketch has a pencil - same with the sample assembly you provided. 

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That is a bug with derived sketches I believe. They show as not fully constrained, but that is incorrect.