Sheet metal – controlling corner gap

I don't think this is possible but I'm going to ask... Does anyone
know a way to control the gap in corners of sheet metal parts using
the edge flange sheet metal feature? As far as I know, the gap is
always controlled by the inside radius. You can change the type of
flange (material inside, material outside, bend outside) which
controls the position of the bend but the gap is still always
determined by the inside radius using this feature. If you use the
miter flange feature you can control this corner gap with a
dimensioned value (if you select multiple edges) but that doesn't give
you options for flanges of different lengths or profiles. You can
also control this gap using a rip feature but this uses the "old
style" of SolidWorks sheet metal. Neither of these options seem like
good alternatives so I'm hoping someone here knows of another.

Steve

 

Have the

nope

 

Sorry I have only found that using a miter gets around this, Hardly an
acceptable answer.maybe try adding a small miter then adding a tab to create
the rest of your flanges. If someone has a better method I would like to
know also. This really limits the creation of sheetmetal parts. Have the
tools for SM been improved in 2005.

Corey

 

not efficient, but you can sketch the extensions inside the edge-flange
sketch.

 

Model the entire part as a one-thickness, but NOT sheet metal part,
using extrudes, etc. Stay away from shells and rips; make your own
reliefs as 'gaps' between faces, and dont add Bends until the last
feature. You be suprised what you can do with this (awkward) method: I
can even model multi-body sheet metal parts, that all unfold, and with
no errors.

 

The edge flanges seem, by nature, not to give as tight a corner as,
say, a shell/rip combo. but it is more flexible.

You can get slightly more tight corners by EDITING the flange profile
sketch.
By editing, I mean to ERASE the one vertical line that represents the
side of the flange and replace it with 2 lines; one that is slightly
greater that your bend radius height, and the next line vertically
the rest of the flange height.

Make your small replacement line start at the same bottom position SWX
gave you for the original edge flange profile; make it taper at
whatever angle it has to
to meet your new "full height" vertical line, which you can now DIM to
a clearance value from the edge flange next to it.

Be aware that you can get so close that the thing will no longer
unfold;
for a trully tight seam AND flexibility, see my other reply ( to your
other post) about creating the part as a 'standard' solid first...

 

I also think this method gives much more control in the way the part is
built.

 

Richard,

In this particular case we are creating a drawer front which has
provedn to run very well through the shop. It has small gaps (.010)
in the corners which don't have to be welded. One flange is formed
inside so the mitre flange feature couldn't be used. The design was
originally created in AutoCAD with sharp corners and unfolded with
SPI. I created a model in SW that generates the proper flat pattern
but required extra features. I was hoping there was a way to create
these tight corners using the standard flange tool. I also considered
creating the model as extrusions and inserting bends as the last
feature but SW would not unfold/fold the part.

Steve

 

you probably already know this. I discovered that you can take
Well, yes, I discovered this as well, and used it; but have always
wondered if it was bug that would someday come back to bite me ...

 

Nice. I wonder why you are not offered to "link to thickness" the "thin dim"
of a thin extrude?

(2001+)

 

I just emailed you a quick sample. See if you can get edge flanges, or
shell/rip to do what this simple model does (and still unfold!)

You'll notice the gap is a linked value, just change one of the "gap"
dims in the first sketch....

 

What is wrong with using mitre flange and editing the flange that is
different you can add more bends to it or take some away. You can unfold
and remove unwanted bends also, to do this you add an unfold feature add a
sketch to the outside surface use the intersection curve tool to extract the
outside edge of the flattened face and extrude to thickness. Now you can
add the bends you want. You will have to supress the unwanted bends in
Flat-Pattern1.

Corey Scheich