Hi, new to the forum.
Building a Cover for a conveyor system. Trying corner piece, which is a 90 degree turn. The cover is split in the middle with a slight bend, like the pitch of a roof on a house. Is it possible for Solidworks to bend this corner? Bending a curved line? Straight lines no problem, but I'm guessing curved lines are no go? Thanks!
Is there a tutorial available on this? I have the part drawn (I think it's correct)...it's a sheet metal part at this point. I have 2010 and 2011. I'd attach the file here, but don't know how.
Thanks.
To attach a file, select the Use advanced editor link in the top RH corner of the reply box.
You can download the SW2012 Pre-release version via the SW portal if you have signed up for the Beta program, also via the portal.
David Dzurko wrote:
Hi, new to the forum.
Building a Cover for a conveyor system. Trying corner piece, which is a 90 degree turn. The cover is split in the middle with a slight bend, like the pitch of a roof on a house. Is it possible for Solidworks to bend this corner? Bending a curved line? Straight lines no problem, but I'm guessing curved lines are no go? Thanks!
You can produce curved flanges (bends) on SW Sheet Metal parts (as show on the attached picture) and define any angle on the bend, the limitation is that at least one face must be "flat". Therefore in your case the only workaroud possible is to do something as show on the seccond picture...
Your Coveyor Curved Cover can be done with SW (any version after 2008) usign Sheet Metal, as show on the following picture...
The "trick" is to do a very small "flat" suface at the top (0.125" wide in this case, but can be smaller). this part will produce a flat state. Attached is a zip file with the part so you can see how it was build.
I'm attaching the file I started...supposed to be 16 gauge. I can add the edge flanges, but should wait till last, so I get the correct angle in relation to pitch. Edges are both 1". Height to center of bend is 2.5". On the right track? I didn't know how to do a flat like you suggested? Anyone willing to assist?
I guess I should also ask...once the part is created in Solidworks, and you Unfold it, do the fold lines show up? Are we able to flatten this object, show the fold lines, and ultimately, cut this out and make it work?
*sorry for so many questions, I appreciate any help you can offer. I understand the typcial square type objects, these curves are giving me a tough time.
Thanks
Good morning David,
You can build your part like Mauricio showed you, double click on the picture and review the feature manager tree to see the steps he took to build it.
What Mauricio did was made a small sweep at the top, converted the sweep to sheet metal and then added edge flanges for the tappered sides.
The part you show in your first picture can't be made in one piece in SW Sheet Metal prior to 2012, however it is listed as a new feature for the 2012 release, where they added a feature called Swept Flange.
Later,
John
David,
On my previous post I atached a zip file with the actual SW part inside, if you open that file you will see how it is done.
The part can be made in ONE SINGLE PIECE in SW 2010 if you do the "trick" (workaroud) of using a very narrow sweep as a "flat base flange" (to use it be able to start the sheet metal building process). That "narrow sweep" can be made very small (the limit is 0.0001"), therefore it will not influence the real shape of the part. On the example file I created a 0.125" wide base flange in order for you to be able to see it.
That "flat" base flange can be done VERY narrow so it will not be see on the finished part, as mention, I made it 0.125" wide so you can see it on the example, but it can be as small as you want (> 0.0001"), open the part attached to the post and on sketch1 change the value of dimension D2 to 0.0001" and do a rebuild of the part, after that you will see that the bend at the top looks as a single bend.
And YES the par will unfold on a single piece and will show the bending lines, etc.
To unfold the part just press "FLATTEN" on the sheet metal tool bar or "unsuppress" the "Flat-Pattern2" feature on the part, however, how accurate the flat shape will be, that is another issue, since in fact, by fabrication process this part can not be done by press bending, this parts need to be fabricated either by roll forming or by stamping and on those process the deformation of the blank material can not be calculated using parameters for "bending", therefore I will recomend that once you get the flat pattern done by SW you actually test fabricate one part and see the results.
That ability has been added to the sheet metal functions of SW2011. Previous versions had to use a regular revolve or sweep, but could not be flattened as a sheet metal part.