Sheetmetal work?!

[Markaj]

Just a general question about Alibre’s sheet metal ability.
Does anyone here use it professionally (ie for their day job)? I spend my day fighting with Inventor trying to keep holes & flanges in line, & the more I’ve worked with it (3 yrs now) the more I’m convinced it’s not really the right tool for the job. Fine perhaps for mass production, but for one offs??
Is there a really good programme on the market for SM? It was so much easier with a drawing board & skilled fabricators!!

 

[lamar]

I use Alibre daily for professional work and I find it to be very easy to use. with sheet metal you need to know your neutral bend axis to get precise parts. I would say Alibre is good for one offs and for high production use.

just my 2 cents.

 

[Lew_Merrick]

Personally, I am offended that the "CAD Industry" has "adopted" the Lockheed K-Factor inaccurate system for sheetmetal design! I learned to calculate the neutral axis offset and the Hertzian contract stress elongation as an apprentice machinist making blanking, forming, compound, and progressive diesets. Other than adding a few values to the Materials properties dataset (Poisson's ratio, Yield stress, and Tangent or Secant modulus) the math is fairly simple. I have designed some serious, multi-bend, close tolerance/fit systems for automotive, food processing, medical, and spacecraft over the years. The work the first time as designed without the "adjustments" required by the Lockheed K-Factor system of guesswork.

 

[JST]

The problem I see is that I have to convert the actual neutral axis based bending to this silly approximation that Alibre uses. I don't use it enough to always remember the conversion, and have to go look it up.

I always used a table, or if need be, calculated the location of the neutral axis. This other nonsense gets my goat.

But aside from that, I like the sheet metal capability, and have used it professionally with good results. Problems with holes etc may be workflow issues. I often find it quicker to set the locations in the main part, and then transfer them to smaller parts using the project to sketch.

I do NOT use the interdesign relations to keep such things co-ordinated, I WISH that worked in a practical manner, but it does not do it for me.

Of course, sheet metal is not generally very accurate, but that depends on the shop. Best location accuracy has been 10 to 15 thou, worst quoted was something over +- 1mm. The latter was just ridiculous, might be OK for HVAC ducts, not for a product.

Anyhow, you have to allow for tolerances, sheet metal is not like machining. Steel work is even worse, but we've been there, and folks here do not agree.

 

[Lew_Merrick]

The problem I see is that I have to convert the actual neutral axis based bending to this silly approximation that Alibre uses. I don't use it enough to always remember the conversion, and have to go look it up.

For 90° Bends it is simple enough. It is when the Bend is greater than or less than 90° that "issues" come into play. It is the K-Factor itself that is the real abortion!

 

[Markaj]

Yes, the bend allowance gripe aside (I am old school here too), my main issue is as JST alludes to, is the problem of getting holes in two parts.
I have quite a reasonable workflow to create a series of parts driven by master parameters, with flanges & holes that line up & fit together nicely, however the problems arise as soon as you start adjusting things. Because of the nature of sheetmetal, holes are datumed off edges or faces, as soon as you change something, you lose the references & spend far too long fixing things.
Interdesign relationships in Inventor as with Alibre are unpredictably unreliable, & bolted connections - any more than three & things get awful slow.
In fact it is the general flakyness & unreliability that makes me question it's worth (I do find Alibre much less of a windup to use). Assuming say Onshape to have been developed 'new' rather than evolved like Awfuldesk Inventor, has anyone had any experience with their sheetmetal?

 

[Markaj]

BTW I totally agree, there should be an allowable degree of sloppyiness in alignment of holes. Sometimes you just have to eyeball it (we are not precision sheetmetal here!).
After all if geometric tolerancing will allow for a measure of parallelism, radial alignment, etc etc, it should be easy to say align two holes but with the axes within whatever tolerance you like. Or two faces to mate within .5 degree or whatever.........if you want to!

 

[JST]

Don't do the holes off of things that will change if you can help it (you know that).

Manually, I always put the locations on the flat pattern, because there I could set the relation of holes independent of the bends. The equivalent would be, I suppose, letting the S/W unfold the part with the holes where you drop them, then dimensioning.

No, I don't do that now either, mostly because I really do not do much with the flat patterns now. Current vendors do their own (we used to get a lower setup if we did them). so I just show the part as it is wanted, and let the vendor figure out how to get there. The unfold becomes a useful thing more for in-house prototyping than for production.

Holes may be shown on flanges etc, or from some datum, depending on what is important. For flanges that attach to a plate, similar to a rack chassis, the contact flanges are all in one plane and the holes are dimensioned to each other, with one setting the relation to the edges. That way the vendor knows what is important, which normally is that the holes line up, even if the outline of the chassis moves around a bit relative to the holes on different pieces.

 

[HaroldL]

Is there a really good programme on the market for SM?

IF you listen to their hype, Solid Edge claims to be the "really good" with sheet metal. At my work we use SolidWorks, started with 2007 and now just upgraded to 2016. I like the way SW uses Bend Tables so setting up a part is relatively easy.

One thing that Alibre lacks and, in my opinion, keeps it from being used in the work we do is that you cannot apply different bend data to individual bends. It is assumed that all forms will have the same bend radius and in some cases that is just not true.

 

[JST]

....

One thing that Alibre lacks and, in my opinion, keeps it from being used in the work we do is that you cannot apply different bend data to individual bends. It is assumed that all forms will have the same bend radius and in some cases that is just not true.

Yes, this is absolutely needed.

It's not the only thing that holds it back from being a full "professional" program, but it is one of many smaller issues.

 

[DavidJ]

You have always been able to set individual bend radii within an AD Sheet Metal. There is no difficulty in having multiple bend radii within a one part, or am I mis-understanding what you are looking for?

 

[JST]

But, IIRC, I think you can only set one k-factor..... which really means just one bend allowance. Bend allowance varies with the bend radius, and the bend angle.

 

[HaroldL]

...you can only set one k-factor...

This is true, the K-factor setting is Global as is the Bend Radius. Although you are allowed a Minimum Bend Radius it doesn't let you change the K-factor of any bend that has a radius other than the Global BR.

Another sheet metal "feature" that needs to be corrected is the flange Width adjustment. If anyone has had an opportunity to use it to extend a flange to be longer than the edge it is formed from you will notice that it extends not only the flange but also the bend region. This is totally useless. The width adjustment should extend ONLY the flange. Until this gets corrected the only way to extend the flange width is to add a tab feature or edit the flange sketch.

 

[DavidJ]

How strange - I can edit the K-factor for each bend separately on the advanced tab for the flange (and it results in a changed unfolded length).

Whilst the Global K-Factor is set, you don't have to use this for each and every bend. You could even define additional K parameters to speed up applying them across a complex design.

I'm not saying things couldn't be improved, but some of the statements made above about what can't be done are less than the whole story.

 

[Lew_Merrick]

Let us be clear here, the "neutral axis" is that portion of a piece bent in a circular arc (sheetmetal in this case) that coes not get "strained" (change in length) by being so bent. It is found from the values of r (inside bend radius) and t (thickness) in as "rho" = t/ln((r + t)/r) where "rho" is the distance from the center of the bend to the neutral axis. That makes the "length" of the neutal axis to be "rho"*""Theta" where "Theta" is the Bebd Angle ,easured in Radians.

That is the simple part of things. The strain created by this bending comes in two forms -- compressive and tensile. They are more easily visualized as OML strain and IML strain. The OML length is calculated as (r + t)*"Theta." The IML length" is calculated as r*"Theta." Thus, the OML strain is calculated as (OML length - neutral axis length)/(neutral axis length). Similarly the IML Strain is calculated as (IML length - neutral axis length)/(neutral axis length). These values are converted into simple stresses by dividing them by the Shear Modulus of the material and compaing the result to the Shear Yield Stress of the material as, without yielding the formed part will spring back and fail to fit properly.

Now, mind you, this is a subject that has been the focus of dozens (if not hundreds) of PhD thesis over the years. In the case of Goosenect Press forming there are also Herzian contact stresses to be accounted. I would be happy to prove the old machinist's adage (about being a sharp as a drill and twice as boring) if there is interest.

 

[HaroldL]

I can edit the K-factor for each bend separately on the advanced tab for the flange

Well now that makes a big difference. As long as Alibre has had sheet metal that little nugget has never been revealed. I don't believe there has ever been anything in the Help about being able to apply individual bend K-factors either. I always understood that the Global K setting was the controlling factor for all bends and never thought about changing it on the Advanced tab.

 

[JST]

Don't be surprised that you did not know. I also did not know, and I am not the least bit shy about looking things up in the help or in the big PDF manual.

I never saw anything about individual k-factors either. And I looked for it. Probably I should have just tried it, but as mentioned, I have not done very much sheet metal recently, and it appeared as if one would just be changing the global k-factor.

I went looking in the help, and found the override, BUT IT IS LISTED UNDER LOFTS. There is also a listing under "base flanges". There is NO MENTION of being able to override the global k-factor under "sheet metal parameters", "setting sheet metal properties", "creating flanges", or "parameters", where you would naturally expect to find it if the capability existed.

Since I was not trying to do a loft, I never looked under lofts. Why should I?

Just another one of the very well hidden Alibre features. (assuming it actually exists for ALL bends, I don't know, I have not yet tried it)

 

[BrianE.Evans]

Having done sheet metal parts most of my life and used the Lockheed K factor for about 40 years , I find that for most cabinet and chassis work and architectural sheet metal , the Alibre bend system is close enough . One of the factors not mentioned here is that a bend allowance is only good for a specific metal thickness , hardness and radius . Blow any one of those and you are not going to get what you thought you were going to get . Lou will cringe when I mention that very often the quickest and dirtiest way to get an accurate bend allowance , is to go to the shop with a 2" x4" piece of the metal you want to bend, put it in the brake with the dies you are going to use, then measure it to see what you got.
I will agree with Harold on the flange width adjustment that does need fixing. Sometimes I will take another cut at that with another sketch then get into trouble when I flatten the part and have to go back and do it the right way..

 

[Lew_Merrick]

Having done sheet metal parts most of my life and used the Lockheed K factor for about 40 years , I find that for most cabinet and chassis work and architectural sheet metal , the Alibre bend system is close enough . One of the factors not mentioned here is that a bend allowance is only good for a specific metal thickness , hardness and radius .

Actually, if you read my postings on the subject, I reference all the relevant variables (thickness, inside bend radius, and shear modulus/yield strength) as needing to be considered as well as the bending technique (form fold or gooseneck die form) in my commentary. I admit to not getting into the (shall I say) "deeper mathematical issues" that (even I recognize) that few are interested in following.