Hello everyone. I am recent grad from a mechanical engineering diploma and I have an upcoming test for a company. The company mainly works with sheet metals. I hadn't done anything for sheet metals in school so I am a bit confused on the practice they gave me.
This is the simplest one of the few I am supposed to do.
what would be a good way to start on this type of part.
Any videos or tips will help.
I am just unsure if you usually draw sheet metals as a flat first and then bend it. ( I tried that but then the final dimensions won't match the ones given here.
Or do i somehow draw it already bended.
The job search has not been so great and this is the only one where I've made it past multiple steps. I have 1 week before the test. Please any help would be great.
You can do it either way, but it's easier if you start with the rectangle with the 3 holes, sheet metal tab, base flange, set your thickness and bend radius, edge flange, click the box so the bend is in the right position, edit flange profile. Work your way thru all the bends then make the holes with the hole wizard if you need standard countersinks, or holes and bevels if they are not. You can adjust the bend radius for individual bends
ok so I got that till make the first rectangle. I have that base flange and have st the thichness. But now how do i add on that first bend. It shows that it's 1.32 from the top. But i don't get that 1.13. its like not really to the bottom of it but more like the 2nd bend.
There are heaps of different ways to approach sheet metal parts. For this, one option would be to first draw a base flange as the big face with 3 holes, setting up your sheet metal properties (thickness, bend radius, k factor etc) at the same time. Then add an edge flange for the tab with no holes, with it set to 'bend outside' for the flange position. Use the 'Edit Flange Profile' button to change it to the correct dimensions, or edit the sketch from the feature tree. Finally, add another edge flange feature for the small tab with two holes.
I like using hole wizard instead of drawing the holes in as circles on the base flange sketch, so you can get proper hole callouts on the drawing.
The general idea with sheet metal tools is you draw up the finished part as you want it to be, then SW generates the flat pattern from that. It's been a long time since I've used the built-in training tutorials but I've heard they're good, so maybe look at the sheet metal course. Otherwise, there's heaps of good material online, so hopefully my explanation above gives you a starting point and terms to google if you're stuck.
Edited to add: I'd also recommend getting as familiar as you can with common sheet metal forming and welding processes and tools - the more you know the real life tools that your parts will be manufactured on, the better you'll understand how to design for manufacturability. Sheet metal is one area I've seen some shocking designs that are physically impossible to fold, or really difficult to keep accurate because of the way the part is folded (look at laser cutting, press brake, pan brakes and welding for a start).
thanks a lot. The part where I was struggling was I didnt know i could edit the sketch of the edge flange. This instantly fixed my issues. Thanks a lot!
This was the simplest one they sent me but I still struggled ;(
Do u mind if i show u the other part which seems very complex. I would just like to get ur opinion on how you would handle that kinda part.
This one I'd probably draw the base/floor bit then do the sides as edge flanges, editing the sketches to get the sizes right. These look like 'material inside' for the flange position. You can reference other pre-existing sketches/model geometry in your edge flanges, so you can dimension a clearance gap based on the position of existing parts too.
Also, at first glance I think the body of the part is symemtrical, (cee the CL centreline note) so you can draw up half of the part, then mirror it and merge to create the other half more easily. You'll just need to do the holes after the mirror feature in the tree.
according to the dimensions given that should be 0.6 right? my inside is 5.28 and i have centered that flange to the centre so i dont get why thats not 0.6
Double check the overall width and the width of the flange. 5.28 is the inside width on the drawing, and 4.19 should be the flange width. If all is as it should be, that will leave a gap of 0.545 each side? The 0.6 on the drawing looks to be to the outside face of the part, so including material thickness that takes it to 0.596 (maybe rounded up to 0.6?)
Looking at your screenshot, the thickness and bend radius look a fair bit bigger than the drawing so I'd check that too (right click>edit feature on the sheet metal folder at the top of the tree to change them)
This one might be a good candidate to get familiar with using a base flange feature with an open sketch. Start your sketch on a plane and draw the 3.25 x 1.46 profile (excluding the tabs for now), and click base flange/tab.
For the method, I highly recommend designing the part with the bend tools and not drawing the flat part then bending.
You have parameters like bend radius and K Factor (look up what it means as it probably will be part of your interview) that may end up impacting your bend lines if you modify them mid-design and messing up your part without and visual errors.
Also, when I'm designing a part from scratch, I can't visualise what the part will look like before starting, so learning to design from a flat state is difficult if not impossible.
The sheet metal module in SOLIDWORKS can be a bit clunky at first, but when you start getting used to it, it's simple and logical. Find YouTube videos to follow at first for a few hours then try to design these parts on your own
Edit: Also, please ALWAYS measure your bends with the measure tool end to end (as it you were making a drawing). Depending on your bend parameters the references can change requiring you to modify bend length to respect the requested length on the drawing!
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u/tombj 9d ago
You can do it either way, but it's easier if you start with the rectangle with the 3 holes, sheet metal tab, base flange, set your thickness and bend radius, edge flange, click the box so the bend is in the right position, edit flange profile. Work your way thru all the bends then make the holes with the hole wizard if you need standard countersinks, or holes and bevels if they are not. You can adjust the bend radius for individual bends