Looking for a method to model complex 3D sheet metal parts that is easy to modify.
Attached is a sample shape.
To model the attached (and for some complex shapes) the best way I would suggest is model as a solid body and then use the Convert to Sheet Metal command. This can make it much easier to change the sheet metal part.
but if you are looking for a complex shape that would be easy to modify. One Method would be the skeleton one, make the solid skeleton and reference the sheet metal parts to it. So when you change the skeleton the referenced parts change according to it. Here is an example of a complex part with the skeleton method. Any ideas on how to make this shape out of sheet metal pieces?
Dear Mike and Ingvar,
Your skeleton approach is too modeling intensive and counterproductive.
.The simpler approach is to use the geometry already modelled to achieve the same effect.
This is done by using the master model approach.
Modelling as a solid is the simplest way to model a lot of Sheet Metal parts. You can focus on the part and not how
you are going to split or make it. This is the second step.
Take the existing geometry and either insert this into other parts and reassemble into an assembly file. The parts line up without the need
The conversion to sheetmetal can be done in number of ways.
This is preferably done in the individual files .
1. Convert to Sheetmetal.
2. Insert Bends.
3. Surface extraction Thicken and convert.
4. Third Party solutions to convert solids or surfaces to Sheet Metal.
5. OverModelling or what you call Skeleton Modelling should be the last option.
Think about it. You have the geometry. Why model it again . The data exists you need to convert only to flatten.
Any updates will propagate more readily. Also if holes or tabs are added in the base master model they reflect in the parts as well.
The attached file is a sample shape, not a solid that I need to convert to sheet metal. I need an approach to model complex 3D sheet metal from scratch, not from existing CAD data.
before the advent of the current sheet-metal tools in Solidworks, the old school way was to create a solid, shell, rip, insert bends. and it still works today.
As you see there are different ways to approach anything you do in SolidWorks. I have done literlly tons of sheet metal layouts and models, so simple and some complex, anytime I do a complex part I would do it the way Ingvar Magnusson suggested, skeleton sketch all the way. One thing to keep in mind when you do a component similar to what you showed - You should have a plane at every flatspot and that plane is developed using a single line and a point.
If you start your part with the sketches locked to lines or points that move, then your entire model is parametric and very easy to change. Like Pankaj mentioned a lot of time, but well worth it if you have various sizes or similar shapes to do. If it's a once and done, then it could be a toss up.
Anyone ever tried the method shown in the attached Solidworks part?
yes, i've used that method and posted examples over the past few years
Using a 3D sketch to control the shape of the sheet-metal part.
I've done similar in the past
You missed the whole point.
You start in a simple part file. Make a model using the techniques you are most familiar with.
Getting the bend angles in all the different plane orientations is intimidating using the sheetmetal tools and more time consuming.
Plus not parametric friendly because you are building it bend by bend or flange by flange.
Solid model it . The 3d sketch tools are again cumbersome and slow. Its point by point. In a solid primitive build you get 6 faces of a cube in one go. A simple 2 d sketch and extrusion depth.
You can then chop at any angle you please to achieve what you call a complex model.
If modelled well and thought thru this becomes the base or the master model.
Everything follows on from there.
Instead of recreating the geometry as in the skeleton approach you use the faces and split the master part file into
a number of part files.
In these part files you use the geometry imported from the master file and manipulate it further.
Its a mind blowing and simple technique and achieves your objectives very easily.
This may need some adjustments, hope it helps
Mike I attached the wrong file LOL
Sorry Joe, I am on SW 2015.
Maybe we have a setting wrong here but when ever I attempt to make a drawing of sheet metal parts modeled in that manner the flat pattern refuses to provide bend lines or bend notes. I then have to manually create and locate bend lines and notes. This is to apt to create errors in my opinion. Having spent most of my time making sheet metal parts I find it faster and less prone to error to model in sheet metal from the start.
Since you are using this core functionality of Sheet metal on a daily basis . You should try this approach.
Ensure that the geometry is being inserted into new parts and then being converted.
You will never have any issues believe me.
If you attempt converting the parts within the master file sometimes issues arise especially when mirror features
or split and pattern features exist in the feature tree.
But this has progressively improved . However this is even true for part files with multi body Sheet metal in them modeled from scratch
using the sheet metal tools only .
The problem that I am seeing here must be something different as nothing that complex was used. Apparently those here before me have been creating parts as simple geometry and then converting to sheet metal. No master sketches from external assemblies or mirrored bodies. It seems that they often have to manually insert bend lines and bend notes in their drawings. Last week I had several parts created this way and finally recreated most of them as sheet metal because I don't want the potential errors that I can see that method of drawing creating. I have attached one of the models that did not give me a bend line for you to see.
Convert the solid body to sheet metal using insert bend or convert to sheet metal .
Then insert the sketched bend.
You will have your bend lines appearing without a hitch.
This part does not require this approach. It is recommended when the part has to be split into
multiple static sheet metal bodies to be linked and matched perfectly at the corners.
Have a great day!!
If you have any trouble with any part just send it . I will flatten and send it to you.
I think the real challenge is not to try and break the code. That's simple. You can make Solidworks crash quiet easily.
Direct the efforts to exploring and making sure that you can somehow get it to work.
Since you've decided to use a tool it's only important to get to know the limitations and workarounds if any quickly.
No point cribbing on what doesn't work.
Waste time on what does work !!!
It will make the whole process more constructive.
And finally a recommendation or a method ultimately has to be viewed in light of the comfort level you have with it.
The confidence that you can overcome the small or big hurdles that you may encounter on the way.
We design and build assemblies in sheet metal running to a few thousand parts typically. This learning is not coming from
a theoretical viewpoint or perspective.
Use what works for you but keep expanding that set of tools. Ultimately you want to get your job done in the shortest time .
Also know that the models may have to be tweaked modified and updated.
Engineering change is a constant. That's when the realization dawns on the limitations of the initial strategy deployed. Quite often as early as
when the model has maybe 8 to 9 features.
Chill and have fun.
Acquiring a new skill set never hurt anyone.
Yes I have asked everyone here how they deal with bend lines when they create them with "process bends" and to a man they admit that they usually need to create their own bend lines and notes. And they admit that it is prone to errors if the model changes. But they do it anyway because that is how they learned to do it. As a rule I start with sheet metal, or on rare occasions convert and then use sketched bends so i have never had a problem.
With the master model I think you are saying that I could make the attached assembly as one part and then split it. That may be very helpful and I will have to attempt this on the next design I create. It would be fun to learn. I have suppressed the items that I don't think would be done in the single part.
Do I radius the corners ahead of time or does SW create them when it converts the parts?
Your comments are well said, the only difference that I have and yes it is a personal issue, as a long time user of SW I tend to get stuck with how I used to do it and turning back the page 10 or more years ago most of these new enhancements were extremely buggy. When you're involved in custom design, how can you charge your customer for 5 hours of fixes when it should have taken 1 hour, because you used a new feature that almost worked or crashed, when it hits your pocket book then you go with what you know.
Now I try to use all the new features if I can.
When looking at flat patterns for in drawings
remember to tun on view sketch's otherwise you cant see bend lines.
view sketch off
view sketch's on
mabye somthing to check
That has been step one.
We do a lot of very complex sheetmetal parts, most are supplied to us by our customers in Solidworks format. Our customers design by creating a solid then "shelling" it to create a sheetmetal representation. Sometimes it's very easy to use the "convert to sheetmetal" function, usually it isn't. In those cases I create a sheetmetal model over the customers solid. I pick the largest flat face and create a base flange. From there, I'll pull edge flanges and edit their profiles to match. Once done you can hide the original file and you have your sheetmetal model.
When we first got Solidworks, I tried to add Rips at the appropriate spots and use the "Covert to Sheet Metal" function, but have found that it's much quicker and easier to design a Sheet Metal model from scratch rather than try and get their converted Solid Model to work properly.
I used to get so sick of trying to get Solidworks to accept my selections as Sheetmetal. But once you learn what the Software expects, it becomes quite easy.
If it's giving you a flat pattern, it will give you the bendlines and bend descriptions. If it doesn't there are a few places to look and confirm the settings. When it happens again, I'd contact your VAR and they should be able to pin point the problem. If not, post it here and someone should be able to help you.
When we first got Solidworks, a long time ago, I dreaded trying to get Sheetmetal to work, always always was bad mouthing the software. Now years later, if I have an issue, I figure it's something I did wrong. I love Solidworks, everything except the new screen colors in 16.
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