Modeling a baseball cap

[LDF09]

I'm trying to model the brim of a baseball cap, like the one shown if you follow the link [http://www.amazon.com/Nike-Tech-Swoosh-Gray-Size/dp/B00HTNOMKU/ref=sr_1_14?ie=UTF8&qid=1435642084&sr...

Do I have to create sections and loft that from back to front? or is there a better way, maybe with surface manipulation. Thanks for any tips.

[Anonymous · Accepted solution]

Hi, probably one of the easiest ways to do this hat brim is what I would call "projected slices."  So I first sketched an arc that we can extrude the brim from in Patch (or alternatively, Create Form) environment.

Next in a sketch that looks down onto the brim, did a Project of the edges of the brim, then did a selection box to select that project geometry and right clicked Break Link so no longer purple/linked.  I then filleted the two corners, and made an arc/circle on the other side, with a constraint that made the circle centered (during all this sketching can turn off visibility of brim surface)

Ok next I did Modify > Split body, and chose the two filleted curves at front of brim, and as you can see, that will extend as a "blade" perpendicular to its sketch, to cut through the brim.

Did the same thing for the back circle, right clicked on each of the undesired parts of the brim and chose Remove, did a Thicken of the brim, and also filleted the front edges.

Now any of the features can be edited by "going back in time", and the model will automatically update to reflect a change that we make!

Just one of many ways to go about it.  Let me know if you have any questions/problems if you choose to try this method.

Good luck!

Jesse

[LDF09]

Thanks Jesse, that's perfect. Now I'll attempt to do it myself.

[cekuhnen]

yep his approach is good.
you can also start first with a sphere for the head then add the front part
and later the cut out in the back.

[Anonymous]

Jesse,

  I need to take you back in time over 5 years no and ask how you did one of your steps from the below post.

  From the first picture on "extrude the brim from in Patch (or alternatively, Create Form) environment." how did you extrude a single "arc line"?  I can create a second arc, link them together and then extrude it, but I can't extrude from a single arc.

  I can make the arc using a single line, but when I try to extrude it, there's nothing to pull from.

https://forums.autodesk.com/t5/fusion-360-design-validate/modeling-a-baseball-cap/td-p/5699108

[laughingcreek]

That first extrude is done in the surface tab, not solid-

[Anonymous]

Not that part, I'm on the second picture:

Next in a sketch that looks down onto the brim, did a Project of the edges of the brim, then did a selection box to select that project geometry and right clicked Break Link so no longer purple/linked. I then filleted the two corners, and made an arc/circle on the other side, with a constraint that made the circle centered (during all this sketching can turn off visibility of brim surface)

  I've got the two circles drawn and made the selection box for the next step, but can't find out how to "select that project geometry and right clicked Break Link so no longer purple/linked" and select the bill portion.

[Anonymous]

I think the big issue are the changes from the version they were using in 2015 and the one I'm using now "version 2.0.8.156".

  I had other life events and issues that made me drop my project designing for a year and now trying to get back at it.  Even before I quit designing I remember the big changes that took place between what I was using in 2018 and the newer version I worked with.

  I found it hard to find different tools.

[laughingcreek]

Not sure which part your having trouble with.  also not sure why he broke the projection link.   seems like that would make edits more difficult.  anyway, maybe this screen cast will help.  small differences in approach, but basically the same-

https://knowledge.autodesk.com/community/screencast/5e49c594-f2ec-4b06-9792-c92f9fbca961

also attached the file

[Anonymous]

Alex,

  That looks a lot easier.  I'll have to try these procedures in my project.  I have a specific project to reduce the size of an existing hat/cap down to 44% of it's original size.  It's not a ballcap, but the technique can be modified to the project.

  I'm even going to orient the bill of the hat to the correct number of degrees from the headband about 33 degrees.  I already have the rest of the hat done, just had problems with the bill.

  Thank you

[laughingcreek]

There is also a newish ruled surface feature that may be of use.  Hard to say with out seeing a model.

you might consider starting a new post and trying to get help specific to what your trying to do.