Sheet Metal, Box with 1 45degree angle

[Jwouters]

I am trying to create a simple sheet metal box. I start off with a square sketch, then I create sheet metal. Now I want to 3 bends to be 90 degrees, and the 4th has to be 45 degrees.

What would be the best method creating such part. The problem I have is that I can't get the corners to be nicely closed (the same way as if it where 4 90degree angles in 1 bend-feature)

I have tried creating a shelled solid, then converting this to sheet metal. The problem with this method is that the 2 corners where the 90degree bends meet, are not really closed.

The attached image should make things a bit more clear.

thx in advance

 

[ArtL]

The first thing I see wrong is the radiuses are not correct. If you have a 1/8R. in a inside corner, then the outside R. should be 1/8 plus the thickness of your material.Not being a "hot rod" sheet metal guy, what I do is make the box up and then flatten it.It seems to work O.K. for me, or at least good enough that a sheet metal shop can understand what I want and deliver a good part.

 

[Jwouters]

The radiuses are giving by our laser-cut company. We send them .step files, so having a good model is quite important. Having a model like the image, would a unsatisfied part

 

[Updraft]

I never really liked making sheet metal parts "from the ground up" using the "add a flange" approach. I have found it much easier (for most, but not all of our sheet metal projects) to model the part as a thin solid with sharp bends and uniform thicknesses. Then I'll turn the part into sheet metal. The sheet metal feature then requires the information of inside bend radius, bend calculation (we use K-factors), and thickness.

The things we have found to be most important in making an accurate flat pattern (and therefore an accurate finished part) is to model using two sets of data measured in the shop. The first of these is the actual material thickness. We had situations where the modeling was done with the published nominal thickness of the material, but the several thousandths difference from the actual thickness had a huge impact. We now use a table for our sheet metal parts that lists the actual thicknesses of the material for our gauges (we check these values quarterly or if we change vendors). The second critical piece of shop data is the K-factor. Since we did our own bending we created an array of typical combinations of thicknesses and bend radii and measured coupons (made from scrap) before and after bending. These measurements went into a spreadsheet that computed the K-factor for those particular combinations.

With these two sets of data our sheet metal accuracy was typically better than +/-.006 up to 8" over two bends (with Cpk>1.3). As a result of this precision we were able to convert several machined components into sheet metal and reduce costs as well as add features/design options. For those parts that were already sheet metal this improved precision resulted in lower scrap and much faster assembly.

- - -Updraft

 

[Jwouters]

Thanks Updracht for the info .. We use an external company for our sheet metal (laser)cutting and bending. We've got a radius table for the various plate thicknesses. The parts we create are accurate enough for our work, so we are happy with this method.

Although my problem doesn't have much to do with k-factors and bend radii .. it's 'just' about SolidWorks and the Sheet-Metal module of it. If you look at the attached image, you see 2 sheet-metal bodies. The right one is pretty much what I want to achieve. I created this with converting a solidbody into sheetmetal. The problem is with the upper corner. I want this one to be the same as the left body.

The lower corner (circle) is the 45degree bend. The 'cut/gap' created with converting to sheet-metal looks pretty good for me. But SolidWorks uses the same 'method' for the cut/gap at the upper corner .. which I don't like. I hope I'm clear about my problem now .

-J

 

[ctopher]

Check out YouTube.

http://www.youtube.com/results?search_query=solidworks+sheet+metal+box&aq=4

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[CorBlimeyLimey]

Try creating the 90° bends (with the 45° ends) before the 45° edge flange.

 

[CorBlimeyLimey]

The Closed Corner function can also be used to adjust how the edges meet.

 

[drawoh]

Jwouters,

I have designed lots of sheet metal boxes. Conversion to sheet metal is just about the last thing I do. The next to last thing I do is to rip the corners. I do not want SolidWorks to sort this out.

Start from a shell or a flat base. Add any sides or flanges you need. Add mounting holes. Move the walls and flanges as your requirement changes.

When you are satisfied with your design, work out how you want your metal to be folded, and rip your corners accordingly. Now, hit the sheet metal button.

After converting to sheet metal, you may want to add flanges with the flange tool. I usually flatten it and add stress relieving radii to the inside corners. Then, I bend it again.

I find it difficult to modify sheet metal boxes. The sheet metal attaches all sorts of crap to your model. The later you apply it, the easier your job will be.

Our vendor's rep likes to point out then when people complain that SolidWorks' sheet metal tool won't do something, it turns out the sheet metal shops cannot do it either.

JHG

 

[DiegoLGraves]

With all due respect, you should take the time to learn the sheet metal features in SolidWorks, then use them as they are designed. They are quite robust. Modeling a solid, then ripping it and converting to sheet metal is a last resort for me, and reminds me of working with imported models 10 years ago. If you learn good sheet metal modeling practices your vendors and other SW users will appreciate it when it comes time to revise or modify your models.
No flame intended; ymmv. Diego

 

[drawoh]

DiegoLGraves,

Often during design, I have no clue of how the part is going to be ripped and bent until the design is mostly done. I flip flanges back and forth. I flip walls and bases around. I move access holes and mount points. This can be extremely messy with a part that has been set to sheet metal and has bends specified. I prefer to not do this until I know what I intend to do.

The sheet metal is powerful, but I can mess it up.

On machined parts, one of the last things I do is apply the fillets for the machining radii. Again, I often do not know how I am going to do this until late on the design.

JHG

 

[CorBlimeyLimey]

As usual with SW, there is no definitive right or wrong way to create a model. SW has many tools to be used in whatever way the user deems most efficient.

 

[StrykerTECH]

Did you try checking on the the "trim side to bends" feature ?


StrykerTECH Engineering Staff
Milwaukee, WI

http://www.stryker-tech.com/

 

[StrykerTECH]

Here is an example

StrykerTECH Engineering Staff
Milwaukee, WI

http://www.stryker-tech.com/