How do you fill in a hole in a sheet metal part?

shawn_crocker

I used to use the tab feature.  I would draw a sketch over the hole and then use the tab feature and it would fill in the hole.  Now, it seems the system is blocking tab from being used in this way.  Also, can't use delete face with the heal option.  I'm feeling surprised there is no way to remove a hole from an active sheet metal model(anymore).

John_P_Desilets

Another option you can use is the move face feature. If you move the face inward you can close the hole. However, you cannot apply an end condition for the move face feature so it can be less stable. 

John_P_Desilets

@shawn_crocker I was able to use the tab feature with this example. Can you try to make the sketch on the opposite face of the sheet metal part and try again?

Cary_Bettenhausen

Create a sketch on the face you want to fill, leave the sketch open and go right to the Tab feature. Click inside the hole(s) you want to fill. Done.

shawn_crocker

@Cary_Bettenhausen
That not working for some reason.

John_P_Desilets

Another option you can use is the move face feature. If you move the face inward you can close the hole. However, you cannot apply an end condition for the move face feature so it can be less stable. 

shawn_crocker

Thanks @John_P_Desilets.  I will use that.  I feel a little baffled that the tab feature used to work and now does not.

John_P_Desilets

@shawn_crocker I was able to use the tab feature with this example. Can you try to make the sketch on the opposite face of the sheet metal part and try again?

shawn_crocker

@John_P_Desilets
Still no worky.  I'm getting the same message.

John_P_Desilets

@shawn_crocker In your video, it doesn't look like you sketched a circle over the hole. Can you try that? In the example I tested, I made a circle and constrained it to the edge of the hole. 

matthew_stacy

Where the heck are these "holes" coming from?  Are these sheet metal models imported files or native onshape parts?

shawn_crocker

@John_P_Desilets
Doesn't work with sketch and constrained circle.  I normally just do a use command on the existing edge.  I started trying with a circle but tried with just an open sketch in the video because it seemed to be suggested by @Cary_Bettenhausen

shawn_crocker

@matthew_stacy
They are coming from a hole feature that has been patterned.  I will often pattern out some holes and then just go back and delete a couple that I don't want part of the pattern.  In the past, I have had no issue using the tab feature to fill in the un-wanted patterned holes on an active sheet metal model.  Of course, I do want this op being done on the active model because I don't want them showing up in the flat pattern.

shawn_crocker

@John_P_Desilets
Actually, I just noticed the move face workaround isn't working either.  The move face feature isn't allowing me to select the face of the hole.  I think this is a new bug or something because I definitely have been able to use move face on hole faces on active sheet metal 

shawn_crocker

@jmoellers
Hi John.  I think this post is related to the ticket #338178.

shawn_crocker

Just noticed it seems to be holes created by the hole feature that will not fill in with the tab feature.  If I create the hole using extrude remove, I can fill it in just fine with the tab feature.

matthew_stacy

@shawn_crocker, the Tab feature seemed to work for me.  Check out this example.  I extruded a single circular profile through the sheet metal flat pattern.  Then I feature-patterned that extrude-cut (to make a second instance of the "hole").

To "fill the hole" I sketched on the face of the sheet metal, and by "sketched" I mean just selected the perimeter of the extra hole and selected project/use <u>.  Then I created a tab feature using this sketch.

Does this approach work for your application?

Another approach that seems to work is to select an edge of the hole and "Fill" to create a surface.  Then use that fill-surface for a Tab feature (Tab 2 in the linked document, above).  Tab 2 is currently suppressed in the model.