Midplane in Sheet metal parts

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.

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

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

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

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?

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 ....