Sketch on Extrusion?

[Anonymous]

Howdy, folks.

Can't seem to figure out how to get this done.  Hope someone can help.

I've been trying to apply a series of holes on an electronics enclosure to provide some airflow.  I was able to make a manual sketch on one side (flat plane) and extrude, but I can't seem to figure out how to copy/paste that sketch to the vertical surfaces.

My workflow for the main housing was to make a sketch and extrude to create a solid body, then apply the 'shell' command.  For the lid, I used the same sketch, extruded to create a flat panel (the 'lid'), then moved the panel to the position you see here.  Once I did that, I used the sketch command to make a series of holes that I copy/pasted and then extruded to create the ventilation pattern.

However, I want those holes to also be on the 4 sides and bottom panel of the main box.  I just can't seem to get it to work right.

Thanks in advance!

[etfrench]

There are several ways to do this.  Here's how I would do it.

1. Use the sketch for the lid to create the holes in the bottom. Use a two direction Extrude if there are other bodies in the way.
2. Create a new component and project the geometry to a new sketch in the component.
3. Rotate the component to align it with one of the sides.
4. Extrude the holes through both of the aligned sides.
5. Repeat steps 2-4 for the other set of sides.

p.s. It's usually better to design bodies in their assembled position,instead of moving them.

p.s.p.s. See Rule #1

[Anonymous]

Forgive me, because I'm new to Fusion and don't have my head around the concepts just yet.

I think the problem with that method is that - as you can see - there are already components residing inside the enclosure.  So extruding in both directions will create buckshot out of my electronics.  And because it took quite some time to create the pattern of different size holes, I'd rather copy/paste the sketch than re-creating it.

I also don't understand what you mean when you say 'make another component' when I already have the housing.  Are you saying I need to have six separate panels extruded from six different sketches?

I'm sure it's just because I don't understand what's going on here, but I was hoping this wouldn't be so hard.  My expectation would have been - from a layman's viewpoint - that I select the circles I want, copy them as a group, flip the view, select the target surface, paste, extrude, and it should be done.  Apparently it just doesn't work that way here for some reason, and it's not intuitive at all.

Anyway, if you have an easier way to do this, I'm all ears.

Thanks!

[laughingcreek]

You can copy sketch entities from one to another using copy/paste.  You do have to be in an active sketch when you paste.  It can be a little tricky also because the sketch entities will paste into the new sketch relative to the origin of the new sketch.  That can be tricky, b/c the origin isn't always in the right spot.  One way to make the process more predictable is to use the origin planes for your sketches.

Here is a screen cast of the approach i would take. (simplistic geometry of course, just trying to show steps).  By way of example, I also used 2 different extrude methods.  The extrude  tool has a lot of very useful settings that are worth exploring.

Also attaching resulting design for you to review.-

[etfrench]

As usual, there are many ways in Fusion 360 to accomplish the same task.  @laughingcreek's suggestion to copy between sketches is probably easier than copying and moving a component containing the sketch.

Here's a screencast showing the component move method:

There are at least four ways to avoid cutting bodies that are in the path of an Extrude|Cut operation:

Turn visibility of the offending bodies off.

Use a two direction extrude.

Use the To and From settings.

Deselect the bodies in the Objects to Cut section of the Extrude dialog.

Note:  The strange behaviour of the extrude command at the 2:15 mark is because I used a Paste instead of a Paste New command when copying the sketch component.