How can I force a body to update after a sketch is changed?

[Anonymous]

Occasionally, I encounter bodies that don't reflect the underlying sketches extruded to create them. This doesn't happen often but when it does, it occurs after I modify the sketch. Unfortunately, except for the scenario outlined below, I don't have additional details on how to recreate the issue. To fix the issue I delete the body and extrude the sketch. Is this really the best approach?

Here's one scenario where I recall this happening a few times. Imagine a sketch comprised of a rectangle (1/2" tall x 3" long) with a 1/4" hole hole placed 1/2" from each end. Save the sketch and extrude the shape to 1/4" thickness and perform other work on other components, joints,etc. Hours or days later, I modified the sketch by a) increasing the overall length to 6", and b) placing 1/4" diameter holes every 1/2" along the length. The body might update to reflect SOME of the new holes but not all. However when the sketch appears as the cursor hovers over it, the sketch appears correctly including all the holes.

Is there a way I can manually force a body or entire file to update / recalculate? Saving and re-opening the file doesn't fix the issue.

[jeff_strater]

it should work like you expect.  Editing the sketch should update the body (assuming a Parametric design).  If you come across an example, please share it here.  We'd like to take a look.  Thanks.

[HughesTooling]

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@Anonymous wrote:

a) increasing the overall length to 6", and b) placing 1/4" diameter holes every 1/2" along the length. The body might update to reflect SOME of the new holes but not all. However when the sketch appears as the cursor hovers over it, the sketch appears correctly including all the holes.

Is there a way I can manually force a body or entire file to update / recalculate? Saving and re-opening the file doesn't fix the issue.

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No Fusion does not work like this, if you add profiles to the sketch you have to edit the extrude and add them.

Mark

[TheCADWhisperer]

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@Anonymous wrote:

Is there a way I can manually force a body or entire file to update / recalculate?

Edit Feature

Ctrl (CMD?) select/unselect profiles as needed.

Done!

Attach *.f3d file here if you can't figure it out.

[brandon.willis901]

I'm experiencing this exact issue right now.  I have a hexagon in a sketch that I've extruded.  I went back and changed the width and height of the hexagon, and when I exit the sketch the solid is the same as before.  It will not update.  It also does not give me an option to edit the extrusion.

[jhackney1972]

Please attach your model, the Forum users, need to see this one.  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section of a forum post to attach it.

[brandon.willis901]

File attached.  I edited Sketch 1 in Carbon Fiber Case and Extrude1 should have updated to reflect the change.  

[jhackney1972]

You failed to read Message 2, of this Forum thread.  Your model is in Direct Modeling mode, not parametric, so it will not update.  I would recommend that you switch to Parametric Modeling, you will enjoy Fusion 360 a lot more.  

[brandon.willis901]

I did see that, but I had thought that all designs were parametric by default.  I didn't even realize that non-parametric was an option until today.  Can I turn my design into a parametric design or do I have to start over?

[jhackney1972]

You are addressing your post to @Anonymous, but I will respond anyway.  You can configure Fusion 360 to start up in Parametric Modeling model using your Preferences.  I have highlighted the entry you need to change.  You must restart Fusion 360 after you change it.  You can recognize Parametric Mode in a few ways but the main one is the Design Timeline will appear at the bottom of the screen.

You can start Capturing Design History (Parametric Modeling) at any time but I am afraid all design history that came before you start cannot be changed to use Parametric design.

[jhackney1972]

You are probably new to the Forum so I will give you a little advise.  If you have an issue or question, you would like to post about, you should not "piggy back" on someone else's post.  Create your own, they are free!  Piggy backing will tend to be ignored a lot of the time and we do not want that.

[brandon.willis901]

Hey, thanks for the advice.  Yes, this is my first time posting in the forum so I really appreciate the help and the advice. In the future if I have questions I'll for sure open a new thread. 

So I went to find that setting and change it to parametric, but it's already set to parametric.  So I'm not sure how this design ended up not being built in parametric mode.  I started by importing a step file and then designed the case around it.  Does it maybe switch to non-parametric when you start with a step file?

[jhackney1972]

Yes, a STP file only contains non-parametric bodies so it comes in in Direct Modeling mode.  If you create a new file you should be in Parametric mode, and you should see the timeline as I mention earlier.  In this particular file, if you right click on the top item, in the Browser, you can choose “Capture Design History” and turn on parametric design from this point on.  It will not affect the existing bodies.

So if you had turned on Parametric design, as outline above, after you imported the STP file and before you designed the case, you would not be having any issues since you case would be a parametric design and the sketch changes would have transferred to the model.

[jhackney1972]

I was not on my computer when I posted my last reply so today I wanted to give you a Screencast of what I was describing in my post.

[brandon.willis901]

Thank you so much!  That video was immensely helpful.  I'm coming from several thousand hours of Catia, and just learning where all the functions are in Fusion has been a chore.  So just watching you work I learned a number of things I didn't know about Fusion.  Thanks a ton!