Attached is my most basic tank design stripped down with no ports and only a handful of sheet metal pieces.
The key features of this model and draft are the following:
1. Every piece of sheet metal is detailed how to be cut and folded (except one that uses another drawing)
2. The overall size of the model is driven by planes X1, Y1, Z1
3. B1 and B2 interact and change if they change thickness and bend radius
4. Everything else interacts and changes if anything changes thickness
The goal here is to be able to re-size and re-gage the model without losing any of the bend table information that takes time to set up.
Also worth note: there are lots of variables used to create flanges that maintain exactly a 1" flange length (from bend line to edge of part) that is not an option when using flange design. This is lots of math for the baffle (F1) where the angle of the baffle could be anything.
Now to the question. Am I missing anything or doing too much work to accomplish my goals? I have tried doing this in Sync, but there is no way to re-size one part from another in sync unless I do a lot more variable work.
As @nanan00 said, I would at the very least be driving the location of the reference planes by connecting them to a skeleton sketch of sorts. But you should look into using a master model that all of your parts derive from. I use interpart copies and simply convert those to sheet metal, it has many many benefits. As to all the bend table info you generate, while it is quite impressive how far you've taken it, I've never needed to get that far into detail. I give the brake operators everything they need which is location of the bend lines and angle of the bend and bend radius. This is all achieved by dimensioning to the bend line in the flat, and then having a simple callout that pulls in the bend radius and angle and direction info. Far simpler.
as already mentioned in PM, I can suggest to try following:
Where do I see the advantage over the assembly and plane/sketch interpart solution?
You only have one single master part with a elativ simple part model to define all You need - most You need.
All children sheet metal parts automaticall gets updated and are placed in the assembly at the origin.
This method allos YOu, to have different materials and sheet thickness for every sheet metal part.
Another approach - what would be my favorite if possible - is to have a multi body PSM with one part body and several sheet bodies in it.
Would be even easier to play with but what is the disadvantage?
All sheet bodies must have the same thickness.
If this is not possible, then this method could not be used.
Give it a try
I just have created a fast test situation and it works great for me
Thank all for your suggestions.
I read up on the multi body stuff from help. That does not work at all because all of the sheets of multi body must be the same gage.
By default I use 10 gage pans, 12 gage walls, and 14 gage baffles. But that mixture is edited depending on the tank size and material (We use carbon, stainless, and aluminum). So each part could be any of on 12 different gages.
One thing I don't understand about many of the suggestions here is how interpart copy functions or placing by coordinates help at all.
Another thing that does not make sense is using sketches to control planes.
I'm using assembly planes to control part sketches. That way I "KNOW" that when I move a plane, that the many parts being driven from it are all using the same reference.
The planes are the only piece of geometry that is, in general, between the coordinate system and part sketches. At least for ordered. In Sync they recently added a cube I would love to take advantage of but can't for ordered designs.
The file is one of about 100 different designs I have, most of them, much much more complex. All must be able to change overall size and change gage with about a 30 min turn around once the "template" has been created. I can now create a template file like this in about 3 hours because I have done it so many times.
Now back to the big picture. How this get's used is the entire set of files (Draft, assembly, and parts) are copied to a new job and edited. By working this way, the design is nailed down other than size and gage, and all of the drafting is done, other them making views fit the pages right.
One detail that will help many understand the model interactions is to edit the gage of B1 and B2 to something thicker. Then update the model and draft file. You will notice the lid changes size to compensate for the body thickness change.
The only thing I have to manually edit in the model are the lid notches, other than size and gage of course.
And of course, every job required different porting, but that another can of worms I'm leaving out of this.
@12GAGEIn reference to the planes being driven by a sketch, all I was saying was, okay you have your parallel reference planes, right? Well in the assembly, just create a sketch on the top plane. Draw a rectangle with it being centered on your base reference planes. Dimension the rectangle to what the outside of your box should be. Then, when defining the parallel planes, instead of keying in a value distance, instead just snap to one of those points on the rectangle.
"One detail that will help many understand the model interactions is to edit the gage of B1 and B2 to something thicker. Then update the model and draft file. You will notice the lid changes size to compensate for the body thickness change."
This same basic thing is achieved by me by editing my thinwall feature in my base model. After I do that, then of course I have to edit the gage of my piece parts, and once it is done everything fits absolutely perfect(on the computer, of course).
Another detail I don't know how I would handle with thin wall design is the baffle setup. I need to push around some math in the variable table that include Thickness, Bend radius, Bend allowance (that I calculate), Inside setback, outside setback. All so that I end up with what I call a 1" flange (not finished height, but distance from bend line to edge of part)
I do know they are trying to add a new flange design option that would allow me to create flanges based on flat distance rather than finished distance.
Where I work, all of the design standard were set up with old school flat design. For example, I will ask for the location of a port. the answer will be x inches from the edge of the flat. The shop wants me to adjust bend locations but not flat patterns. CAD does not work that way. In CAD, the flat pattern is the result not the cause. Unless you make the part by flat sketch, then add the bends later. But that is very difficult to blend together with a re-sizable assembly.
@12GAGEI agree, the goal is the final product. This is why I hate it when customers send us drawings that have almost no info on the formed part and most the dims on the flat pattern. Should tell me where you want things to be when it's done, not where you think it should be before we form it, on our brake, with our punches and V-dies, with our K-factor. If they want to be able to reject the finished part for not fitting, they need to tell us what it is supposed to be when it's done.
I agree nominus38. I have to explain that I want finished dimensions not flat patterns to document a design.
The problem is, the shop has flat patterns programmed into a punch and plasma as the ONLY place the information is available. The real kicker is that bending turns out different if the part's grain was cut with or across the bend.