Unable to select face

[markandcandyingle]

I am working to design a replacement arm for a pair of Costa sunglasses.  I have the arm 90% complete but I need to add a hinge to attach to the frame.  For some reason I cannot select the face where I need to draw a rectangle sketch to extrude for the hinge.  This drawing is my second version and I was able to select the face on version one after clicking on the Sketch icon.  Below is a screencast video showing what is happening.  The hinge needs to be perpendicular the face.....I am really frustrated since this is a basic step in Fusion 360. I have done it many times before.

Does anyone have any ideas about what is wrong? Or what I am doing wrong?

[etfrench]

You're clicking on the Line Command on the Sketch toolbar, instead of the drop down. Is the Create Sketch command available on the drop down menu?

If you right click on the face, is the Create Sketch menu item available in the context menu? 

If the answer to either of the above is yes, create the sketch. 

If you draw the end view of the hinge on this sketch, then you can extrude it. After this you can create the side view and use the Extrude cut command to finalize the hinge. Use the Look At command to make it easier to draw the hinge.

Alternatively, you could create the hinge shape as a new component and use the Align command to put the hinge in the correct position.

[davebYYPCU]

Not sure but I am thinking you are not asking to create a sketch,

The grid highlights and is not the plane you are looking for,

You should be able to Create sketch then click the face on the end of the arm, continue from there...

When you click the line command and then that face, it should start a sketch, so it may not be a flat face....

might help

[markandcandyingle]

So maybe thats the issue....I may not have a flat face.  After highlighting the face and selecting the Sketch command, the face is not selectable.  I guess I need to start over.  Not sure what else to do here.

[Mike.Grau]

Hi @markandcandyingle,

Thank you for sharing the Screencast.

Could you try to create a "Plane" at the face and create a new sketch on that plane?

I hope this helps.

Thanks,

[davebYYPCU]

I would not be starting over, 

your face does appear to be flat, but it is not on a parallel to any origin either, 

so how did you make that face, I can see two extrudes, two fillets, a symbol I don't know in the timeline, but no construction planes

if you already have a sketch to make that face, you can do another profile for the hinge, in the same sketch,

if that does not work then you might have some bug that the file will show up.

[markandcandyingle]

@Mike.Grau Yes I added a plane to see if it would help.  I was able to draw a sketch and extrude but then I could not add a draft angle.  There needs to be a slight angle to match up with the frame.

[markandcandyingle]

@davebYYPCU I have attached an archive file for you to review.  The face was created from a Patch workspace extrude, then I add the fillets on either side.

[davebYYPCU]

I am away from Fusion the rest of the day, so will check again tomorrow, (Sat afternoon now), sorry about that.

Can you make your extrude large to be intersecting with the frame, too look right, then be trimmed by the frame itself?.

[etfrench]

Here's the worlds worst hinge.

Instead of creating the hinge object, it would be best to fix the face on the frame by cutting a few microns off the end. There is something wrong with it as the Combine|Join doesn't work after the end of the video. Shaving a little off of the frame body seems to cure the problem. Just offset the line projected from the frame a few microns. Create closed boundary and Extrude|Cut it from the frame.   After this you can create the hinge as in the video and the Combine|Join will work.

[markandcandyingle]

@davebYYPCU No rush on this so take your time.  I am more interested in understanding what I did to cause the problem.  It appears the face was not flat but I am not sure what caused it....I am "self-taught" in Fusion 360 so I fear there is a fundamental piece I am missing.  I started over keeping everything parallel to the x-axis when possible.  That seemed to help because I was able to complete the design.  Below is a screencast.  I will use the mirror function to create the right arm.  Also attached is a picture of the Costa sunglasses with the broken arm.

[davebYYPCU · Accepted solution]

Gooday Mark,

Found it, the end "face" of the arm was and is unslectable, we knew that, because it is not flat "to the system".  You and I figure it must be flat,

the reason is apparently coming from the construction of the arm itself, either

sketch 11 is a 3d sketch, (can't tell if the vertical line is a spline or line)  a 2d sketch might fix it, didn't go that far.

or the Intersecting extrude

or the thicken,

or the conbination of both,

technical gurus might figure a more detailed "why"

The fix is to trim a sliver off the end of the arm, I got it down to 0.012mm to make it work.  I used Plane on a path, 0.012 from the end of the spline curve, (sketch 10)

Split Body, with that Plane, then hid the sliver body, the sketch would then work by selecting the new plane or face.

There other ways to "face" the arm,

An analogy - on a lathe you would normally face the material in the chuck to be true before the / any other operations,

[markandcandyingle]

Yes that was it!  Awesome work Dave!  Now I know that I need to keep edges straight and parallel when doing my sketches.  I really appreciate your time investigating the issue!

[etfrench]

Hmmm. You must not have watched the video I posted....

[davebYYPCU]

Yep, @etfrench saw your video, no problem there, we have both used the same fix

but the op was looking for the "why isn't it flat" I am tending to think the straight line for that face maybe a spline in a 3d sketch, a primary cause,

Not detracting from your video, our Op has moved on past this problem as a result.