SW 2008
I create part one (1)
Mirrored part (1), call it part (2)
Than crated part (3) that joins both parts 1&2
Part 1&2 are parallel and flat, 1” apart.
Part 3 is a half of a pipe, created by two arc’s.
This half of a pipe joins the edge of part 1&2.
I then created part (4) that just joins part 1,2&3 as one
Question;
How do I turn this into sheet metal so I can flatten it for a pattern.
I’ve used the Base tool then tried the bend tool on 1&2 where they meet 3
But all I get is errors.
You should be able to select one of the faces of Part 1 and Insert>Bends. Make sure all your material thicknesses are equal.
Not having a picture, your parts seems that it was created very "round-about". Perhaps you can redraw your sketch profile instead of joining all these different parts? It would make for a more robust model.
Sorry I’ve been converting from Autocad architectural.
I was waiting on another post to save it externally
Thanks
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you zipped the wrong file. anything with a tilde (~) is just a temporary lock to indicate the file is open.
I think it was because I had the drawing open
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i missed the 2008 statement. anyway i created the part as sheetmetal, no joining.
the flats need to be tangent to the arc.
and as jeff mentioned a relief between arc and tabs.
Not having any luck with your method, it won’t allow a tab to be made from the half pipe shape. I also extruded a part off the edge of the half pipe and that doesn’t work either.
I think I’ll just go out to the garage and cut it out of construction paper, that will take less time. Wish AutoCad had an unfold feature.Thanks for your time though.
It just seems to take forever to design stuff in SolidWorks
it's just a matter of learning how to use the sheetmetal features.
see jpeg's. not to scale.
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That look great, it wasn’t a question of whether it could be done though, I know it can, just don’t know the process.
I’ve tried it both ways now creating the half pipe then making the flat tabs, didn’t work. Creating the flat tab first then the half pipe, didn’t work. The only thing that almost worked so far is I used the Hem tool, set to 1” and 180* but now I can’t figure out how to create the other tab out of sheet metal…
see attached.
after opening parasolid file in 2008, select vertical edge at rear, then insert> sheetmetal> bends. you can get a flat-pattern at that point.
if you attempt, as a starting point, sketch U, then insert> sheetmetal> base flange.
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Rebuild error; You must select a fixed planar face or a linear edge on an end face of a cylindrical face.
if you attempt, as a starting point, sketch U, then insert> sheetmetal> base flange.
Error; The sketch plane for the tab feature must coincide with the base body’s top or bottom
Rebuild error; You must select a fixed planar face or a linear edge on an end face of a cylindrical face.
if you attempt, as a starting point, sketch U, then insert> sheetmetal> base flange.
Error; The sketch plane for the tab feature must coincide with the base body’s top or bottom
ooops, i meant to say select "face" then insert> sheetmetal> bends
i was temporarily distracted by another thread relating to a cylinder.
i attached a zip file of jpegs as a step by step guide, just 6 features.
the base flange sketch is just a single edge profile.
the thickness is set by the base flange feature.
look closely at the feature tree in each jpeg.
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As mentioned above I did try that, in fact I’ve tried multiple ways starting with a “U” and half pipe. If I start with a U it wont let me add tabs to the back edge or extrude cut without making most of the part disappear. Similar to this method;
http://www.solidworkstutorials.com/2009/09/tutorial-22-how-to-create-u-bracket-sheetmetal/
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When you create the initial part, put the sketch on the front plane with the center point of the arc coincident to the origin. Dimension the arc and the legs. Create the base flange feature. Open a sketch on the right plane. Draw the triangle profile, and a rectangle that will cut from the top of the arc to the tangent line. Cut-extrude 'through all' in both directions. Open a sketch on one of the flat face and draw the profile of the tab. Base flange/tab feature. Mirror using the right plane.
I'm on 2010, or I'd post the part.
Reno,
Here is an example part for you. One of numerous ways to build this part in SolidWorks.
Of course it is easier to use the old cad system to create the part. You have been using it for how long, years maybe. Remember when you first learned the old cad system. It was probably hard back then to.
SolidWorks will get easier to use when you learn what it needs. You have a lot of old thinking to flush from your brain. After a while SolidWorks will be just as easy as your old cad system is to use.
Cheers,
Anna
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Dear Reno,
Since you are working on an Autodesk product you have a lot going for you.
Your'e transition into Solidworks is going to be easy. Use the 2D command emulator to use the same commands as in Autocad.
A radically different approach to solving your problem is by using the following method :
Forget Sheetmetal Modelling its overwhelming initially. With all the settings etc.
1.Import the side view sketch of the hinge from AutoCad into Solidworks on to the front plane of a part file.
( A simple CopyClip procedure )
2. Extrude it to the depth required.
3. Fillet the front end.
4. Shell the solid body by removing the faces not needed.
5. Insert bends and your done ( A sheetmetal conversion tool )
.
When using sheetmetal please note that a single open loop sketch is sufficient it does not have to be a closed loop.
A closed loop generates a sheet which cannot be unfolded . A crucial 1st step error. Not uncommon especially if you've worked
with 3d in Autocad or Architecture.
Since extrude is the most intutively and widely used first command ; this is the way to go. Plus you get to use the geometry created
in Autodesk .
But believe me the inital approach taken by you indicates that you're not the one for conventional ideas. You're part in part join was
way out man ?!!!!!
Pankaj Bir
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Thanks for all your help, suggestions and tips. I wish I could just upload "how to use SolidWorks" directly into my brain..LoL
I hate the time it takes to learn new programs.
I figured out a way that worked later that evening, much! later…
I think the process sounds similar to Jeff Mirisola's second suggestion.
What I did was create a flat piece of sheet metal and mirrored the triangular shapes to opposite
sides then put I bend in the center and added tab portion with the two holes after.
I printed it out 1:1 used spray adhesive to attach it to construction paper than cut the shape out and transferred to 12ga sheet metal, cut that out, drilled the holes
then made some dies for my air/hydro press to shape it into a U.
They turned out great! Tomorrow I'll weld them to the frame and test it out!
Thanks again