Can anyone explain how the 'flex' command works? It does no ask for a K factor so how does it figure out the proper flat pattern?
As far as I know the flex command was not meant for sheet metal.
It has too many rigid commands in it.
Do any of these explain it?
Not sure, cant download or watch 'youtube' at work? By back figuring it looks like it uses the inside dia to figure out the flat, not adding any aditional stock. If this is the case the flat will roughly be off by pie times the stock thickness? Which in my case is more than a half inch short. Should we not be using 'FLEX' commands to design sheet metal ?
I think that many of the features outside of the sheet metal tools are fair game so long as you avoid any freeform tools like flex and deform. I find these incredibly useful: move face, shell, rib, holes, extrudes, and also the surfacing tool sets.
I've used Flex for things like labels, to wrap the label to a radius that matches a surface.
...Chris, you are talk about the flat pattern being off, but the flat is whatever you start with. There is no actual flat pattern option for a flexed part is there? You just suppress the flex, right? Since you can bend, stretch, etc however you like it would be up to you to match the flexed version to how a material actually behaves.
The flex tool works great with sheetmetal you can bend, twist, but its mostly just eyeballing.
So are lofts, domes, redundant configurations and inserting parts within parts.
I use all of these too because unfortunately at the end of the day, my end product is a two dimensional drawing that goes out to fabrication, and an exploded dxf that goes to the plasma table.
Sometimes you just have to make it look pretty on the drawing and throw parametrics out the window.
Like others have mentioned, the Flex command was not purposed or is suited for Sheetmetal since you can not unfold a flex - not to mention other issue with it which simply don't apply to sheetmetal. If you want to know more about how to use it pass the SW online help, Charles Clup has a video about it on his SWTUTS site here
OK, I am trying to make a cylander with a top lip. I can do this with the FLEX command but it doesnt behave like sheet metal and the EDGE FLANGE command doesnt work for me on the rolled edge of the cylander? How would I model this and be able to unfold it without the FLEX command?
I think you will be able to do it in SW 2012. I don't think I would trust the flat pattern dimensions.
Well if you don't need an accurate flat pattern you can do it already, with SW 2010.
*Make the tube with a sheetmetal Base-Flange. Leave a split in the tube.
*Add the lip with a normal sweep. Bit tricky to get it to sweep all the way around, had to have the split line up with the profile sketch.
I tried it out and It flattens out, but it ain't right.
The profile of the lip is about 15mm long and my flat pattern only added 5mm of material.
If the lip is made with a tool that deforms the end of the tube then that complicates modelling the part.
The SolidWorks Sheet Metal features are for parts that are done on a brake press, or simple forms and wipes, where there is no stretching or compression of metal in 2 directions. Cheers, Anna
The SolidWorks Sheet Metal features are for parts that are done on a brake press, or simple forms and wipes, where there is no stretching or compression of metal in 2 directions.
Is there another way to make the lip in real life? Seems like the flat pattern would need a bunch of tears in it, to approximate the curve. (image from experimenting with sweeping the lip, sweep profile in purple)
There's lots of good ways to make this part in real life. You can either have it spun as one piece at a metal spinning shop if you can't tolerate a seam, or you can bend the lip onto a rectangular panel and then roll it and seam weld the joint. The second approach also provides logic that will work toward generating a valid flat pattern as well.
In my experience, in parts with compound bending (bends across bends) you have to fake it in the model by applying some logic. I'd use 3 configurations in this model to keep track of the steps. A default configuration, a configuration with the gradual curve flattened out, and an actual flat pattern. Using this case as a fairly simple example, I'd first calculate the rolling length of the long curve (bend) by modeling a part with no lip and using a k-factor of 0.5, and model a configuration with lip that is rectangular and of the length you calculated for the curve. Then I'd make a flat configuration where you calculate your bend dimension of the lip and the body as your width, and the previously established length. Obviously in this case the flat profile is rectangular, which makes the math a little easier.
I've done this before a few times with non-rectangular profiles and it gets a lot messier than this, and then involves an english wheel to form the part.
See the attached file, I've done what I think I saw in your picture with some assumed dimension and bend deductions.
I've been meaning to look over your interesting reply more. When I went to download your sldprt I realized it is in SW2012, and I'm still on 2010.
So I upgraded my eDrawings to 2012 to at least view it... no luck, I guess you have your settings so that you save without tesselation data (Doc Properties >> Image Quality), but apparently that also means we can't view it in eDrawings.
Anyway, thanks for the explanation. We will go to 2012 someday.
Version mismatch strikes again! Try this E-drawing of the part. This should help.
Edit: Apparently E-drawings doesn't show the feature tree, so this is less help than I had hoped.
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