i have already made some flange in my drawing and how can i make the left side of the flange longer than the base flange. in the pic you see that the drawing must extend to the centerline but how?
My first thought is to create a sketch and make a split part. Try extending that section, then re-combine the bodies.
Not in 2016 version. In 2016 you can exceed the base flange width.
Re: Hello, i have a question about sheet metal.
I do it by extruding from the side. There may be a better way--I'm not a big sheet metal God.
This is what I would do also. Edge flanges can't, in my experience, extend beyond the edge of the parent body.
I third that
In pre2016, You can extend an edge flange by editing the sketch like as shown. You need a small bit lined up with the edge of the base flange.
You can edit the sketch under each edge flange to angle the side out so that each edge flange get progressively wider at the top. This can mimic the taper you are showing. It might actually be better to model the shape as a solid with the outside exactly how you want it then convert to sheet metal. This will reduce having to keep up with so many edge flanges. Using all separate edge flanges will make it difficult to adjust if changes are needed.
If you want to extend it all the way out to the left you can add a BASE FLANGE/TAB to the first flange and then your subsequent edge flanges will go out there as well.
Another way is to use a base-flange/tab so you stay within the sheet metal tools. While this isn't a must, I occasionally run into problems flattening sheet metal with extrudes in them.
If you're using a laser you won't have any problems with tabs that right up to the bend line, but if you're using a turret punch you'll need a tool the size of the gap you created. In this case it's .084. We don't have a .084 punch so the second screen shot is a .120" tool (bigger than I needed but it was hard to see smaller tools). The angled edges are created by SW from the bends, our shop ignores these,
If i use tab it doesnt extend the edge flange, you know how to also make this piece longer? you cant select the edge with the option.
It would be nice if it worked that way, maybe you could request it. You have to sketch the shape you want on the flat surface of the sheet metal. It's basically an extrude to the thickness of the metal. Like this.
A lot of work arounds are explained above, but SW2016 makes it much easier to have a wider flange than base flange.
In SW2016 simply add your flange and in flange property sheet, click Edit Flange profile button and drag the sketch to width you need, click Back button and then green check mark. you're done.
Can you upload the part you are having trouble with?
sure, look at the Original post, as you can see at the end of the buck i have only extend the straight sides, but i dont know how to extend the edge flange
Instead of extending, try making the part a little longer and trim both ends perpendicular to the top flange, I think that's what you are trying to achieve.
I'm a release ahead of you, so you may not have a way to open my version of your part. So I attached a couple of screen shots, and a parasolid too.
It's hard to see but the sketch follows the top flange, and at each end drops perpendicular to the top flange.
Then make a cut as shown.
Also, I would have made a part like this by making half and then mirroring the body, half the Edge-Flanges.
Heyy, yeah i made the it over and made the basic sketch longer, and in the end i cut the right size of the drawing. what you suggested. Thanks for helping
Ok Hylke,, See if this works for you. I rolled up just after Base-Flange1 and added a 10mm boss on to the end of the base flange. This extended all edge flanges to the left. Then I used your Sketch56, dragged it to the right to meet up with you original base flange edge then did a cut extrude to slice off the left end. Your base flange is still the original length. I suppressed all the tabs and additional unfold and fold. The part flattens as it should. Attached a 2014 file.
Best Dennis, made a new (longer) buck of it and at the end i extruded cut it. At the first place i did that alson but got an alert of problems because he didnt want to extend the base flange. when i did that i got problems with all my edge flanges so that didnt work out, but rather by your drawing it worked? how?? thanks for helping
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