Sheet Metal-Flat first then fold or Folded first then flatten

[MikeKovacik4928]

In the context of what I am doing, converting all 2d autocad drawings to 3d inventor.

Therefore the folded part has been cut and bent umpteen times.

Is it better to

1. draw the final shape and then flatten it or

2.  draw each flange and then fold it.

I am thinking which would give the more accurate result, at the end of the day,

There is an existing autocad 2d drawing of the flat pattern, and an existing autocad 2d drawing 

of the folded part. Obviously in autocad the link between the 2 is at the discretion ot the drafter 

and his production team, whereas the link between the 2 in Inventor, is set by the software and 

your settings.

In inventor the 2 would be linked by the sheet metal defaults, which I usually leave at the inner bend 

radius the same as the sheet metal thickness.

I haven't had the experience of actually matching the bending of the model to what the brake press

(not CNC but the old manual type where you place the piece by hand and line up the bending line by eye) and brake press bending tool does (?the radius on the nose of the bending die??)

What are your experiences and advice out there

Mike Kovacik

Inventor Pro 2020 ; Vault Pro 2020

South Africa

[WHolzwarth]

I think, in the end you want the finished part look like the drawing of this state.

I'd create the folded part at first, after that the flattened sheet. The flattened look can change with the selected k-factor, set as default of 0.44. I don't think, placing the bend line at the inner edge of the bend (k=0) is really a good choice.

[MikeKovacik4928]

Betreff

Thanks

I have decided to do just that, create the folded part first as a plain .ipt, to the dimensions the finished product is 

supposed to be, and then worry about the sheet metal and sheet metal settings after, ie convert the ipt to sheet metal and then unfold it and develop it as necessary

From my perception, it makes more sense that way

Mike

[WHolzwarth]

Sometimes starting with a basic IPT may be necessary, when geometries are difficult. But you need to set bend shapes by yourself. Starting with a sheetmetal template can make it easier in most cases.

Conversion to Sheetmetal is needed in any case, for getting the flatpattern.

[mcgyvr]

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@MikeKovacik4928 wrote:

Betreff

Thanks

I have decided to do just that, create the folded part first as a plain .ipt, to the dimensions the finished product is 

supposed to be, and then worry about the sheet metal and sheet metal settings after, ie convert the ipt to sheet metal and then unfold it and develop it as necessary

From my perception, it makes more sense that way

Mike

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@MikeKovacik4928  You may want to adjust your perception... 😋

Starting with a sheet metal template first gives you immediate access to flange creation tools that are necessary for modeling up formed sheet metal parts,etc...  There is little to no reason to start with a standard part template. 

[Frederick_Law]

My part template default to sheet metal.

Which way you start depends on what do you want.

Are you only recreating old drawings?

Will you make any change to them?

Lots of time the flat is done by trial and experience.  It could be more accurate and sometime impossible for CAD to recreate.  The flat might have been adjusted to work with specific tooling.

In this case, you'll need to cheat the flat.

Or create a bend table instead of using K-factor.

[Cadmanto]

I agree with @mcgyvr .  You want to start with the sheet metal template.  If you have Autocad drawings, you can always import the sketches into the model sketch and then use the Contour flange tool to create the shape.  Then after it is modeled you can easily create the flat pattern.  My 2 cents.  😊

Windows 10 x64 -16GB Ram
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Inventor Pro 2020

[Anonymous]

 I have more than 10 years experience in such things, I used to dive in them deeply.

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@MikeKovacik4928 wrote:

..

Is it better to

1. draw the final shape and then flatten it or

2.  draw each flange and then fold it.

I am thinking which would give the more accurate result

---

Generally doesn't matter with the same settings, length of pattern will be the same.
But if your goal to have a good model and a good flat pattern for it the best practice is to create model first. This is the most accurate way. If you'll do all correctly this will work on all equipment and dimensions will be very accurate.

On some plants you may have one flat pattern which dictates everything. For instance you may have a cutting line and you can't modify the pattern. In such situations maybe would be reasonable to unlink flat pattern from model and store them separatly as 2 documents.

There maybe several nuances which depend on logic of things you're doing, you goals, geometry, tools.

As you intuitively began to work with creation of model, go ahead, probably the logic is correct and this is the right way.

How to get models precise:

You need to know what parameters to use in what situations and what they are for your tools.

If you have only 90 degrees angles you may use BD (bend deduction) parameter instead of K-factor. It maybe useful because you'll have always precise numbers. And one important point - that it doesn't depend on radius in you model (but depends on tools). Also you'll have precise numbers. It might be important if you sometimes need to calculate them recisely without CAD system. BD depends on the tools and thicknesses more than k-factor.

If your angles are different, you need to use k-factor. It is the most common parameter. I'd recommend to use k-factor almost always.

BUT to have correct results you must to define what the k-factor is. You need to bend materials of all thicknesses you use on your plant on all tools, and measure what is k-factor. It doesn't depend much on radiuses.

As I remember on the last plant I worked the k-factor which fits all thicknesses was about 0.273.

As you understand that the flat-patterns you'll get will be slightly different from what you have in the meantime because your ones will be more accurate for production your equipment. You also may calculate bend parameters based on current drawings. But there still be some error of rounding numbers.

As I said there is few nuances but generally the best practices depend on your goals.

[Anonymous]

Hi MikeKovacik4928,

For ease of editing the design, I recommend modeling the folded part then flattening it. Being at a custom fab shop means having to edit designs a lot.

Historically, the K-factor at my work is based on experiment. I work at a place that does lots of stainless steel sheet metal bending. We were fortunate enough to get a brand new Accurpress brake. During the training we learned that each material/punch/die combination will have its own K-factor. It is overwhelming to envision capturing them all (gotta catch em all?). One way the representative suggested to solve this issue was to have a flat pattern generation software capable of sheet layout called Radbend. What is great about this is that it takes your finished, folded part and flattens it just right, taking into account the material/punch/die. It also works with Radan, our sheet metal nesting software. What is bad about it is that it means Inventor's generated flat pattern is going to be wrong every time. If you're like most people, you don't really have the funds to get a new press brake and new specialized software to deal with this issue. You will most likely have to experiment to get your K-factors.

[andrewiv]

I had a colleague of mine explain it this way - We are designing the final piece not the flat pattern, the flat pattern is what is used to make our design.  Whenever starting a new piece I use this philosophy.  However, we also have some parts that are drawn in AutoCAD and if I am not changing the piece, just redrawing it in Inventor, I will usually start with the flat pattern and then fold it.  This way I make sure that what they will build does not change from what they have built.

[swalton]

We model the formed shape.  

The only people who care about the flat shape are the laser cutter operator, the QC inspector, and the press operator. 

Everyone else in the production, spares, warranty departments and the end customer cares about the formed shape.

[Casey.P]

@MikeKovacik4928,

There are multiple ways of doing this, as you have seen. Since you have older AutoCAD drawings that have both the flat and formed state already drawn, you could use a contour flange in a sheet metal sketch when converting everything over to Inventor. This is really helpful if you have one or two flanges. But if you have more than two flanges, then you'll have to model the remaining either using flange or bend. 

Often times at my company, we deal with customers who will send us drawings with the final formed product detailed. If you take a look at the file attached, I took the following steps to create the Inventor model:

 1) set my sheet metal rules accordingly (.035 material, .4 K-factor)

2) Create a contour flange based off of the sketch that I created.

3) Create my feature cuts as needed.

4) Create my A-side definition

5) Create a flat pattern.

The only time I would use the bend or fold options is if I knew without a shadow of a doubt what my K-factor is for the type of material and thickness the part would be made out of. However, even then it is sometimes difficult to avoid the number of bends and unbends and bend backs to get to the final product.