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Create a hollow trapezium

ogama

New member
Hi guys,


Im trying to create a hollow trapezium in sheetmetal, but I'm having problems blending the corners. The two long sides has a different angle than the short side. (See picture below)


Any good technic to build this part.


BTW: The part in the picture was buildwith an extrude-draft and shell feature, but it can not be true that I can not make it in sheetmetal. Hope you can help me


View attachment 3946
 
i would have made it in solid with blend feature and then converted it into sheetmetal. later adding rips and all that stuffs....
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From what you have described, I understand that you wish to create a sheet metal part that is bent to get that shape.


I suggest you make an extrude feature (solid), give cuts at the ends for the trapezium, Shell (for removing the surfaces and giving uniform thickness) and then convert to sheet metal (Applications>Sheetmetal...).


Conversion to sheetmetal takes care of edge rip, bends and corner reliefs.
 
Thanks guys,


That was what I ended doing. I gave upand went from solid to sheetmetal.





Thanks for your comments
 
It sounds like you solved it, but I'll give my additional thoughts.


Solid and convert is the way to go. I've gotten very nice closed corners by adding rounds to the solid before the sheetmetal conversion.


First, round the edges where the bends will beusing thewall thickness + the inside bend radius.


Then round the edges where you want joints using the wall thickness.


After conversion, use a surface rip to remove the 1x wall thickness round surfaces where you want a joint, including the corners.


You'll be left with a nice, clean and tight joint that should unfold (assuming the rest of your geometry does).
 
dgs said:
I've gotten very nice closed corners by adding rounds to the solid before the sheetmetal conversion.


First, round the edges where the bends will beusing thewall thickness + the inside bend radius.


Then round the edges where you want joints using the wall thickness.
I didn't quite get it. You can add bends during conversion. You can specify either INSIDE or OUTSIDE bend radius and that is it. You can also perform an edge rip at the edges, add corner reliefs... all during conversion itself.
 
Not a conversion feature, which I think is what you're talking about, I mean going to the Applications menu and selecting 'Sheetmetal' within a solid part. Then select shell, pick your remove surfaces and enter a thickness. After it's converted to sheetmetal, you add in surface rips (which just remove the selected surface) to take out the 1x wall rounds.
 
What I mean is you need not add rounds before the conversion (i.e to the solid). Rounds in the form of bend radii can be added during conversion to Sheetmetal from Solid.
 
Really, how? I've heard of such but when I convert using the Applications menus, I don't see any place to do that. All I get is picks for shell/driving surface, remove surf (for the shell) or surface pick (for driving surf) and then enter a wall thickness. Where in that process would I add bend raddi? In my experience (limited, honestly) this also endds up with a 1x round on all sharp corners, which I guess could be used for the surf rips later. (Is that what you mean?)
 
This should explain... Create a solid...shell in solid...Applications...sheetmetal..


You will be prompted for a driving surface and a sheet thickness = shell value...


Then click on the Icon shown to get the dialog box open...


View attachment 3962
 
SRINIVASANIYER1 said:
This should explain... Create a solid...shell in solid...Applications...sheetmetal..


You will be prompted for a driving surface and a sheet thickness = shell value...


Then click on the Icon shown to get the dialog box open...


So, that then creates a separate 'conversion' feature, right? Or does it somehow edit the 'first wall' feature created by the initial conversion to sheetmetal?


I think I played with that once but found the prompts and dialog boxes less than intuitive, so I gave up.


The terminology is confusing since there's a conversion to sheetmetal and an actualconversion feature. At least I think there is.
 
What the initial conversion does is to define a Driving surface and ensures that a uniform thickness is defined. The part at this stage cannot be unbent.


With the second conversion feature you can define the Bends, Corner Reliefs, Types of reliefs, Edge rips....all in the same command.
 
I got it. Sounds like a little more streamlined way of doing it.


Still, having a the actual sheetmetal conversion be listed as a wall and have the conversion feature separate (and not actually available until after it's been 'converted') is a bit confusing.


BTW - I'ts mid morning (10:00 AM)here in Ohio, what time is it in India?!?
 
You guys sure make this simple-looking part sound difficult. I haven't studied the Pro/E sheet metal package yet, but I know this is a 30-second task in SolidWorks sheet metal (part of their standard package, at no additional charge).Also, solid modeling operations are easily interlaced with sheet metal operations to create features.
 
Ditto in Pro|E.


Sheetmetal is included with the basic package, you can combine solid and sheetmetal together to a point (solid geom must be done first)and, although it sounds hard, I bet I could do it in close to your 30 seconds.


I bet if you described the steps in SW (in this level of detail), it might sound hard there too.
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