Sheetmetal - Curved Edge as base for flange

[cdub]

Sheetmetal - Curved Edge as base for flange

I designed some small sheetmetal parts, and found it very annoying that the base edge for all sheetmetal flange features must be a straight line.

The sheetmetal integration in any other CAD package I've used has supported selecting curved surfaces for flanges.

This is something that really should have been present at the first release of anything that was going to be described as a "sheetmetal" tool

 

[jwknecht]

Maybe they should call it "Sheet Metal Light."

I don't have any experience with other packages, but I have tried to use the Alibre Sheet Metal on some projects. The only use I have found is unfolding some simple shapes to find the flat pattern.

If you get much beyond a basic box, it won't do.

I would like to see more from the relationship with Amada http://www.alibre.com/news/pr/pr20050711.asp

 

[cherkey]

I beg to differ...I've come up with some nice designs that probably qualify as more than just a 'basic box'.
cherkey

 

[jemmej]

Me too!

Can you bend on a curved piece? I am not a sheet metal house so I don't know the answer. The only way I can see doing that is if you are using a process other than bending such as drawing. We use the sheetmetal package for all of our enclosures. Are there some features that could be implemented? Sure. Is it crap? Hardly. Very useful and the main reason we purchased a pro license.

Jim

 

[jwknecht]

My critique is not meant in a bad way. I am hoping to see improvment in the software. There are many sheet metal applicaitions that Alibre is not the correct tool for. This does not mean it is not the right tool for you. I am agreeing with the poster that we need enhancements (this is the enhancement section).

 

[jemmej]

I suppose a few of us who use the package a lot took offense at this...

If you get much beyond a basic box, it won't do.

The original poster would like a flange on a circular edge. That's fine. Its an enhancement request. I just didn't like your basic box coment!

I've done much more things with sheetmetal than this I assure you.

Cheers!

Jim

 

[jwknecht]

I am not the one that originally said that comment. Actually, when I was getting tech support from Alibre, the tech support person told me that.

 

[jemmej]

LOL! Well, that's rich! Then again, the tech support person probalby knows about all the silky smooth improvements in v9!

No offense taken really. Its your opinion (and other's apparently!), you are entitled to it. Though I like the sheetmetal now, I'm looking forward to v9!!

Jim

 

[cdub]

"bending" on a curve

I will go out on a limb, and say that you physically can not put a curved "bend" on a part in the sense that you are thinking (with a brake). I hate to say can not, so maybe at the very least we'll say it's not a good idea to do so. I'm not a sheet metal forming house either.

Typically though, the sheet metal package of a CAD tool is flexible enough to aid in describing parts with geometry that would need to be formed by drawing.

Yes, with the "solid" CAD tools (shell, etc) you could create the finished part geometry of a part like this. Typically, using the sheetmetal features is quicker than using the "solids", as things like reliefs and radii are handled in a more automated way.

Even though the flat pattern of the part may not be terribly accurate (constant thickness assumed), it is very handy for several things (estimating, blank size, etc).

 

[Jimpulse]

>>I will go out on a limb, and say that you physically can not put a curved "bend" on a part in the sense that you are thinking
>>(with a brake). I hate to say can not, so maybe at the very least we'll say it's not a good idea to do so.


I'm not sure I understand what you're talking about....
"Curved" bends are VERY COMMAN in manufactured parts where tooling/Equipment is not limited to Press Brakes. Its not only a "Good Idea", it is a necessary and well accepted process. I cant remember the last time I saw an automobile that could be built using a press brake.

I would like enhancements to the Sheetmetal package to include DRAWN and FORMED part representation with flat part generation.
I am not designing cars but I do draw blower housings with inlet venturis etc. I'm aware that i can (and have) design these sheetmetal parts using solid modeling features in conjunction with the Sheetmetal design package but that sort of misses the point.

 

[cdub]

curved "bends"

Yes, I understand how common it is to design something with a curved bend.

My only point was that once you put a curved bend into your design, you are departing from having the part made only on brakes. This is important if you are in low volumes, one offs, etc....

As it stands today, the alibre sheetmetal package seems to more or less reflect what can be done ONLY with a brake. Thus, I am asking for the ENHANCEMENT of having CAD features that more directly reflect geometry creation beyond what we have today.

 

[HaroldL]

Flange on a curve

Following this thread, I thought I'd give a try at this as an exersize. Given that the inlets for this type of blower are a drawn or stamped component, Alibre can model them, but without any way of flattening for a developed blank.

I am not designing cars but I do draw blower housings with inlet venturis etc. I'm aware that i can (and have) design these sheetmetal parts using solid modeling features in conjunction with the Sheetmetal design package but that sort of misses the point.

Jimpulse, take a look at this link, is this what you are designing? (Please excuse my attempt at this if it's not quite up to snuff.)

http://www.alibre.com/forum/viewtopic.php?t=1963

HaroldL

 

[rbrian]

Blower shape, flanges on curves, and tricks...

HaroldL - I see the blower - nice job for a quick forum reply! It appears to me - you skipped the flanges on the sides/ends and instead just put in a dimple with cout out on a nice large circle there - is that right? And - the rolled shell - is basically from what I see - flat flange + large radius flange + reversed flat flange (at the outlet side of the blower).

Now - I have made - with some effort in the past - a poly-sided, short triangular flats, Sheet-metal Cone (or cone-like) structure. [It takes quite a while with each flange - needing to have it's sketch carefully edited to become a triangle]

I have not been able to use the sheet metal normal tools to create a flattenable flange on a curved edge yet - however - that curved edge - CAN be used to become a path in a Sweep - to complete the stuctural effect - of having a flange 'Formed' onto the multi-curved edge.
For an existing example of this - see: http://aircraft-computational.com/alibr ... index.html - go to 'helidev' and look at the rib. Robert

 

[HaroldL]

Blower flanges and design

Robert.

For the shell, my base feature was a flat tab. I then added a flange and selected "Bend Only", I keyed in a large bend radius and guestimated the angle at about 270 degrees. The last flange I toggled the "Bend Only" option off to get a flange, keyed in the smaller bend radius and angle to get the flange parallel the the base panel. The holes in the flange are sketched cuts made after an "Unbend" operation. I sketched on hole and patterned the cut feature to give me the spacing along the flange on the first direction and the second direction puts them on the other side. Then I put in a "Rebend" to roll it back up.

I then went back and edited the large radius bend to fine tune the degrees to get the final flange to the proper distance for the opening height. I suppose the may be an easier way to find the angles, but with tweaking I got the outlet flanges to be parallel.

The ends are basically two dimples. I started with a sketch that was .220 larger than the inside dims of the shell. I then projected some reference geometry to the sketch plane and checked the "Maintain Associativity" option. From the ref geometry I created an offset of .220" and used the sketch to create the first dimple to a depth of about 1.00".

The inlet venturi is another dimple with a 6.00" diameter, depth is .699, the die radius of .600" and "Cut Out Material" is selected.

I used Extrude Cuts to trim off the base flange and the end of the outlet portion. The holes in the edge flange were Extrude Cuts also, one set for the flat portion and a pattern off a rotated plane for the curved flange. I had to play with the planes' angle to get the right spacing to match the holes in the ends. I was in the assembly context to do the adjusting.

I wanted to use a pattern of dimples with the material removed (for an extruded screw hole) instead of holes but Alibre won't do it, you can't sketch on a curved surface.

I tried to simulate the drawing/stamping process as much as possible, with the draw/trim. It's nice that the dimple feature will let you define your shape to something other than round or square. I've been able to use some odd shapes to form a dimple, but you have to be careful with the angles and radii of the sketch.

Too bad I couldn't mirror the completed part. That would have saved me a lot of time modeling the opposite end. I tried but Alibre froze up and gave a error code. I didn't write down what it was but I don't think Alibre liked what I wanted it to do.

Harold

 

[Anonymous]

To mirror that part you need to do a "save as" and in the new part use the scale function and enter a -1 in the box for the plane you wish to mirror about. This is how you create right and left parts in Alibre.

 

[Mibe]

Keep in mind that the mirrored part is not syncronized with the original part unless you first use a "Boolean Join" of the original part and then scale that with value "-1".

This way the mirrored part will keep up with the future changes in the original part...

 

[HaroldL]

Blower End Piece

Mirroring the part would be nice. But I read somewhere in the Help Manual that Alibre does not mirror sheet metal. I tried with no success.

HaroldL

 

[Mibe]

It mirrors the part if you use the method of "Scale" but it won't work to mirror individual flanges etc.