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Sheet Metal Part
2

Sheet Metal Part

Sheet Metal Part

(OP)
I am trying to make this part using sheet metal functions (or convert the sweeped part to sheet metal).  Forgive the two links, I am new to posting pictures and testing it out.

http://img152.imageshack.us/img152/7985/drippan6qa.gif

[url=http://img152.imageshack.us/my.php?image=drippan6qa.gif][img=http://img152.imageshack.us/img152/7985/drippan6qa.th.gif][/url]

The part shown is a sweep consisting of one end being:
2" across, 2" down, 2" across, 2" up
and the other end being
2" across, 6" down, 2" across, 2" up
The sketches are 32" away from each other.
I would like to convert, or remake, this part into a sheet metal part so I can flatten it.

RE: Sheet Metal Part

(OP)
Here is the corrected linked thumbnail.  I should have used preview the first time.

RE: Sheet Metal Part

Look into "thin feature loft".  I have modelled a part recently very similar to what are looking for.

-Shaggy

RE: Sheet Metal Part

(OP)
Thanks for the reply guys.

Shaggy:  I said sweep, but I meant loft.  I created the two end faces and then lofted them together.  The part lofted is exactly what I want, but I am really trying to learn how to use sheet metal functions properly.

CorBlimeyLimey:  My company won't upgrade SW because I am the only who uses it.  So I couldn't open your file.  I really was hoping for a description of the process, if possible.

Here is what I have so far.  Please correct me if I do something stupid.  I am starting from the top.

1.  Create a sketch on the top plane of a rectangle 2"x32" and use the base flange tab button.  Make it 1/8" thick.

2.  Select the right line and use the edge flange button.  Make it 6" long and adjust the corner properties.

3.  I cut the bottom far corner to get the taper (using extrude cut with a sketch of a triangle).

4.  Another edge flange 2" long.  I adjusted the relief type to a tear and selected extend.  This is to remove the notch on the far corner.

5.  Finally a last edge flange 2" long.

Everything is good except step 5.

Step 5 creates a flange at an angle.  I need the sides to be straight up and down (Like the loft) so I can weld a mirrored piece on the far side and a wall on the near side.  The only way I know around this is to make the original part longer and cut the ends off.  Is that my only choice, or is there another/better option?

RE: Sheet Metal Part

concerning the sheetmetal functionality, you can edit the sketches of the flanges.  This should allow you to correct the problem with the "angled flange" you mentioned in step 5.  It will also allow you to eliminate the cut operation in step 3.  If you edit the sketch created in step 2, you can have the taper in one shot.

For this part, I still prefer the thin loft option.  You will end up with one feature in the tree to control all of the geometry and when you Insert>Sheetmetal>Bends, you get all the functionality of the flat sheet metal (bend radii, and flat pattern.  Since the way you describe the part as such & such on one end and a different such & such on the other, it seems natural to use the loft.

-Shaggy

RE: Sheet Metal Part

(OP)
Thank you, editing the sketches worked real well.  I had a question about converting it to a sheet metal part from a loft.  When I try to do it with insert bends, I get this.



This is why I thought it would be better to do it as sheet metal to begin with.  Do you know why it is showing like this?  I have tried inserting bends and selectin various faces.  I get this result with the top face and left inside faces.  I get errors with the others.  Is there something I am missing?

RE: Sheet Metal Part

There are multiple ways to get what you want using just sheet metal features.  The easiest to explain is as follows:

We'll start off by making the odd angled face and the single flange off of it.  Make a 2" blind extrusion (standard extrusion, not sheet metal) of a trapezoid, 32" long on the bottom, 6" tall on one side, 2" tall on the other side.

Shell out the extrusion 1/8" thick, leaving just the faces you want (front trapezoid and top flange).

Insert bends from your sheet metal functions.

Now pull an edge flange off the bottom edge of the trapezoid 2".  Do that again at the end of that flange to form your last face.

That's it.

You may notice a slight "nub" at the end of the bend on the tall side of the trapezoid that you don't want.  You can add a standard extruded cut on the face of the trapezoid to whack that off if it bothers you.  To get the exact flat pattern of that final cut, you'll have to edit Flat-Pattern1 and uncheck 'Simplify Bends' to process it correctly.

Windows 2000
P4 2.40 GHz
Video Card -  
  Manufacturer: NVIDIA Corporation
  Card: Quadro4 900 XGL/PCI/SSE2
  Driver: 6.14.10.7184

RE: Sheet Metal Part

I was mistaken earlier about thin feature loft.  Look into "lofted bends" in the solidworks help.  This command allows you to complete the part with one feature containing two sketches.

The command is located in Insert>sheetmetal>lofted bends.

-Shaggy

RE: Sheet Metal Part

Psst sloth4z [whisper] Give these guys a star since they have taken the time to help you out.  They have gone past lip service and actually built the model to help you.  These guys will be more willing to help in the future if they get some recognition for there time. [/whisper]

Flores
SW06 SP1.0

RE: Sheet Metal Part

(OP)
Thanks Guys.  I really do appreciate your help.  Looks like there is yet another reason to update.  Apparently SW2001+ does not contain the "Lofted Bends" feature.  Maybe I will get it for Christmas. :)

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