Midplane in Sheet metal parts

I am still using SolidWork 2003, so this might be different in 2004.
Why cant I insert a sheetmetal base flange with a midplane? After
create a sheetmetal part with no bends, i have to manually create a
midplane. Even then, equations are funky, since i get rebuild errors
sometimes when I make an equation for the plane, thickness/2. I know I
can do a stanard base flange, but I dont think thats good practice on
a sheetmetal part.

Any suggestions?

 

I'm not really sure I understand your question. I started a sketch on the
Front plane, sketched a rectangle with a diagonal construction line tied at
the midpoint to the origin, and inserted a base-flange via the sheet metal
toolbar. So, the result was a base-flange with a midplane. What did I
miss?

WT

 

i'm on '04 (and it has extrude mid-plane), but as far i can remember you
could extrude with mid-plane

 

What I think he wanted was for his "base face" to be halfway thru his
stock width. While one can make an EXTRUDE in both directions, one
cant make a BASE FLANGE in both directions.

But that still doesnt give him a base face halfway thru: BASE FLANGE
automatically "picks" the fixed face for unfolding based on the
sketch/plane used to create the base flange, and (mid plane) EXTRUDE
requires you to select a face when you turn it into sheet metal.

In either case, Solidworks ends up using an outside FACE, and not an
arbitrary
distance into the solid ....

 

damn, this reading between the lines crap is tough work. i'm never gonna
get it right.

 

Are we talking about the same thing? I need a midplane that is half
the material thickness. If I draw a sketch on the FRONT plane, and do
a Base-Flange/Tab from the Sheetmetal toolbar, etc doesnt give you the
option one how to extrude it, only the direction. Therefore, you dont
have a midplane that is half material thickness.

This has been like this forever. Does 2004 have this option ?

Here is a screenshot of the base-flange/tab window, and also of the
resulting part.

http://img.photobucket.com/albums/v154/3eleven/SolidWorks/solidworks_sheetmetal_baseflange.jpg

http://img.photobucket.com/albums/v154/3eleven/SolidWorks/solidworks_sheetmetal_result.jpg

 

Are we talking about the same thing?


not likely.

 

start with a thin-extrude (sketch a "single" line segment and extrude), then
insert sheetmetal feature.

 

That wont work, since the part doesnt have any bends in it.

This seems like a oversight on SolidWorks. Why wouldnt someone want
the plane you sketch on be the midplane of your material? Seems like
other people would be complaining about this also.

 

Maybe I'm missing something here, but I don't see the benefit of sketching
new features on the mid-plane of an extrusion. If you add a hole/cut, don't
you then have to do a bi-directional cut? You won't be able to use the hole
wizard, because it doesn't offer the option. For sheet metal, why wouldn't
you want a "real" face to define as your fixed face from which to unfold
bends? How about skectched bends - I don't think they would work from the
mid-plane.

I don't think it's so much an oversight as it is you trying to do something
unusual.

Richard

 

That wont work, since the part doesnt have any bends in it.

yes it will, it dosen't matter that no bends are present.

i concur with richard, i don't see what you're after.

 

If you need to reference the midplane add a reference plane select a surface
and the midpoint of an edge this will put the refplane at the midplane of
the base flange. As everyone pointed out what is the purpose of having a
midplane in this case.

Corey

 

start with a thin-extrude (sketch a "single" line segment and extrude), then

Actually, it does. (or at least "Insert Bends" does).

Solidworks will complain, but then add the Sheet Metal Feature anyway.
Been doing it that way (when I *had* to, not my parts) for years.

 

exactly.

the user should notice that after applying sheetmetal feature (even with no
bends), that all of the tools on sheetmetal toolbar are now active (no
longer grayed out).

 

Thats exactly why I need a midplane on some parts. If I have a plate
(plate1) and I want to weld another plate (plate2)perpendicular to
that plate, but in the middle of it, then I need a midplane (half
material thickness)for plate2.

I never thought about how the sketch plane for the flat pattern, so I
guess thats why SolidWorks doesnt give you the option for miplane
extrustion.

I like your solution, Corey, since it doesnt involve making a equation
for the plane (material thickness/2) i dont like using equations
unless absolutley necessary.

I dont need to use this often, so making a manual plane using the
above is what I will do, thanks

 

Maybe you don't actually need the plane you are thinking of. Obviously I
don't have the whole picture, but can you use the existing midpoint directly
with the midplane of the other part in its other direction, instead of using
the midpoint to create another plane? Kind of working the other direction.
A picture from you would certainly help.

WT

 

Thats exactly why I need a midplane on some parts. If I have a plate

after all of this ... it sounds like this part has no bends.

so out of curiosity, if there are no bends, then why do you need a
sheetmetal feature?

 

so out of curiosity, if there are no bends, then why do you need a
While I cannot vouch for anyone else, I basically *demanded* in my
work that any sheet metal parts that required manufacturing be
created with a "Sheet-Metal"
feature.

I do high volume CNC programming for Punch/Laser/Plasma, (several
hundred programs a day for 3 shifts in 3 facilities) and the only way
I can keep up is to automate the process... I basically need to "Nest"
and toolpath an assembly of flat patterns in minutes. The automation
requires all ambiguities be removed, and the combination of
Sheet-Metal feature and Custom properties define the only ambiguity
left in a valid Swx model (at least for what I do), the actual
Material to be used.

In addition, it provides the following benefits (again, at least for
me)

1) On parts that have no bends, there is no extra work required in
design when compared to an extrude; and Solidworks often 'remembers'
the stock thickness, and therefore using a base flange instead of an
extrude may often be one LESS mouse click.

2) When I search an assembly for parts to include in a nest, I am not
including any non-sheetmetal parts; and therefore not trying to
generate a flat pattern for, say, a PEM fastener.

3) Parts that may actually BE a sheet metal part but whose geometry is
simple enough to be made in, say, a manual shear can be IGNORED by
creating it as an extrude.


So if its Sheet metal, and its unsuppressed, its getting automatically
manufactured ....