How to scale only one face?

[Anonymous]

Hello! I am very new to Fusion, and have a question about scaling faces. It would be nice if the fillet tool could take two radii so that the fillet could be ellipse shaped. So I'm trying to get around that limitation.

What I'm doing is scaling the object in one axis, and then I want to scale the center face smaller. You can see in this diagram. The outer object is there for reference. The inner object is the one I'm trying to change. If I could scale the blue face smaller, I could get the effect I want. But whenever I try to scale the face, the whole object gets selected and scaled instead.

The effect I'm going for is that of a shallow depression that isn't steep. I want the curve to extend further into the object. If I could just scale the selected face smaller, that would fix my problems. I know I have somewhat fixed my problem already by scaling my whole object in one direction. But it isn't enough. The blue object needs to be the same size and dimensions as the enclosing object, disregarding the fillet:

Thanks for any help, I've been struggling with this for a long time.

Edit: I realize that I could fix my problem by increasing the radius of the outer corners of the box. But I don't what those corners to change.

Henning

[Anonymous]

Yeah...

[davebYYPCU · Accepted solution]

Sure, there are 3 sketches, but could be done with one.

I used your base sketch, one on the top of the block, and another for the floor level.

I used a floor (filleted) rectangle just to show that it doesn’t have to be an offset shape.  You can adjust the shape with dimensions.

I used a Loft to make the cutting surface, for the dish.  

Split body with the cutter, and hide the offcut.

Making the cutter, Loft will make the 1/4 job, and use Mirror to duplicate with the origin planes.  When using Loft from the edge of the floor, you can have the tangent result with the click of a drop down menu, for me much easier than cut and fuss with sketch articles.

Many ways to skin a cat, this is just one way.  

But solid Loft as cut is probably more appropriate, having slept on the problem, got side tracked on the corner flow.

Might help.....

[Anonymous]

Ok, I'll see if that makes sense, LOL. Thanks!!! I'm going through some Fusion 360 videos to understand it better. I seem to have gotten where I did (product almost done) by the seat of my pants without understanding some of the basics.

[TheCADWhisperer]

---

@davebYYPCU wrote:

Many ways to skin a cat, this is just one way.  

But solid Loft as cut is probably more appropriate, having slept on the problem, got side tracked on the corner flow.

---

@Anonymous 

So what was the solution?
I got lost on the description of your true Design Intent.

Do you have a photograph of something similar that already exists in the real world?

[Anonymous]

The accepted solutions shows (mostly) what I wanted. I did not, however, figure out how to do it myself. But I thought that it didn't deserve not to be accepted just because I don't know how to use the app.

[davebYYPCU]

I have just answered the PM, didn’t know you had answered here at the time.

Will get you there.

[davebYYPCU]

Check PM.

[TheCADWhisperer]

---

@Anonymous wrote:

...shows (mostly) what I wanted. 

---

What is the difference to needed to obtain exactly what you want?

My attempt attached.

[Anonymous]

Thanks guys. I don't want to have you thinking I'm ignoring this thread, but I can't look at this stuff right at this instant. I will, though, because this is high priority. Just give me a day or two...

[Anonymous]

Okay, I got a chance to look at this today after all. It is very much what I'm looking for, but I would like to take the plane in the bottom of the bowl and move it downwards a bit. How do I do that? When I try, I can't move it down at all, and moving it up (not that I want to) actually changes the top profile curve.

[Anonymous]

Yes, this is very much what I want. How do I move the bottom of the bowl down without changing the top profile curve?

[davebYYPCU]

If the Whisperer used an Offset Plane, Edit the depth, in his model, with new distance on his sketch plane for the floor, but I fell in the trap.  Either way is is editing, no need to start over.

Sketch 5 is on a Mid plane.  That will need changing to an Offset Plane, 

is going to break some stuff, (I shoulda used the offset plane in the first place - dang,)

Do not Delete sketch 5, it is used for the Hole.

you have 2 choices  - move the timeline marker to left of the Midplane, Delete all to the right side of the timeline marker, and rebuild the model, or just edit the file with the following steps.  

Move time Line to in front of the Mid Plane (left side of it).

Make an Offset plane at correct depth.

Make a new sketch (7) on this plane.  

Move timeline with right steps, and Edit Each feature, select, then Right click.

Edit the patch, to select the new sketch profile.

Edit the Loft and reset it to the new Patch edge.

You might find the split body still works, not sure, but reset it if it breaks.

If the holes are still in the middle, the rest will update.

Might help....

[davebYYPCU]

I take that back, just revisited my file, 

Make the Offset Plane, floor thickness from the origin plane, 

then move up to the sketch 5 in the timeline, and select, then right click the icon,

select Redefine Sketch Plane, select the offset plane, 

The file updated without error. 

(Sketch articles changed to green, shouldn't happen but always does, means you lost the purple projected status)

Might help....

[Anonymous]

Oh wow, that worked. I say wow because I thought I'd mess something up. Actually, maybe I did. Because the holes moved down too when I reset the sketch plane for the sketch. And I can't figure out how to fix that. I tried to move the 'master' hole upwards but it didn't work.

What I did to move the bottom of the bowl:

I created the new offset plane, and then I moved it before Sketch5 in the timeline (otherwise I wouldn't see it for the next steps). Then I moved the timeline marker to immediately after Sketch5, and then I right-clicked on Sketch5, chose "Redefine Sketch Plane", and chose the new offset plane.

Is that all correct? Why did the holes move?

Edit: I tried moving the dot in Sketch6 but I couldn't.

Edit2: When I chose "Break Link" for the dot in the sketch, I could move it. Doing so moved the holes in the side just fine. Is that okay? Do I need to re-establish the link? What was the link to?

[davebYYPCU]

Oops, 

When I did not get yellow broken icons, I did not double check the hole location, so yes that is no longer correct.

I had projected the hole centre from the floor level, or more accurately the old floor level was on the mid plane, we changed it, and the hole lines up with the new floor level.

So the fix is to unlink as you mention and add dinensions to the hole point to locate it. 

Or make a new sketch on the new offset plane, (would need the projection from sketch 2, but will break the model by loosing all the work from the patch through to the split body), so quicker to dimension the hole point.

Sorry about that....

[TheCADWhisperer]

---

@Anonymous wrote:
Do you have any guidance on how to create this? I'm looking at this and don't know how you did it.

---

@Anonymous 

Are you still working on this?

I was going to create a video on a simplified technique - but you seem to have abandoned this thread?