My first post here...
I am learning the sheet metal tools and have a drawing with a feature I don't know how to draw.
There is a jog in the part (circled in red). How do I model that? I guess I could use a sweep flange, but is there another way?
You need to create a sketch bend, but use the jog command.
Starta sketch. Draw a line in line w/desired jog dimmed at 50mm (keep line length within part width) and create start the jog command.
Adjust the jog parameters as required to start locate it at the dims shown.
It may default to 45° which may be too steep for a 7mm offset, so just increase the angle.
This will lengthen the overall of the jog but only 50 and 7 are required.
did this as a trial, but it isn't working. where am I off?
Create a base flange that's 16 x 60 long (you can add length later).
Once you've selected a thickness, open Manage Equations and edit the 16mm width to subtract the selected thickness
(because your on;y width dim includes the separate bottom plate.
Start a sketch on the correct side of the metal and draw a line within the width of the part and dim as shown
Start the jog command using the line and the correct fixed face.
Set the offset to 7 and review the other parameters for your requirements.
Here's the jog.
BTW: I don't suggest you do SW sheet metal as is done with "regular" solids, like extruding a profile edge as mentioned here.
Most of my metal rework is from clients doing sheet metal like they're solids.
Since you can model pretty much anything in SW, it's common to see models that can't be realistically fabricated.
With the inherent limits of sheet metal, this is even more true.
Stick with the sheet metal tools for the best sheet metal models, plus you'll actually learn SW sheet metal with habits that will scale with model complexity.
There are SW sheet metal tools, such as "Convert to sheet Metal" and "Insert Bends", that are best for conversion and only used as a "last resort".
I agree with J. Mather, you are selecting examples beyond the "beginner" level.
This may be because these are all that's available to you for examples, which is fine, but keep his words in mind and try to pick out the simpler exercises from them.
That is probably too complex of a part for a beginner, and I do not think it will flatten.
Can you attach your *.sldprt file here?
Confession, I don't even know what I am looking at.
Is that one part or is it an assembly?
Here it is, hopefully.
It looks like it matches the bottom portion well, but as Ned Hutchinson posted, the bottom I believe is one piece and the jog portion is a second piece.
I'd model these as separate sheet metal parts and then assembly them (probably as a weldment).
Also, to further your sheet metal prowess, I recommend using the "Break-Corner/Corner-Trim" tool in sheet metal instead of the std fillet command.
You'll as you do more sheet metal, that you can model something that Break-Corner can't (won't) do. That's a flag.
This how i interpreted it.
I wouldn't use the jog feature, just draw the jog and base flange it.
I was hoping there was some solution that would also apply here;
If I'm reading this drawing correctly and the 20mm wide triangular profile runs the length of the part, this would be a stamped part.
The junction of the two 88 wide jogs and the R4mm bend isn't formable.
See if this thread can help you...
Sheet Metal jog offset less then material thickness?
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