First off, I want to say thank you to thoes to answer questions here. I have been helped much by the responces here.
I'm trying to determine how to create "adjustable" sheet metal parts. When the part is adjusted, the size of the flat pattern and end part is changed. This appears to be compleatly different than the well covered stretched spring adjustible part.
Have any found a good way to use sheet metal as an adjustable part?
I'm already doing adjustible sheet metal by using planes to control the model. But this forces each part to be created within the context of the assembly. Now I'm trying to find a way to have adjustible part that can be used in many assemblies.
To explain the "plane control" over sheet metal, I'm using the following process. (ordered)
1. create assembly, Offset 3 planes so that 6 planes that define the 6 sides of a box exist.
2. create sheet metal part. Start a sketch on one of the planes. Include the 4 planes that ore normal the that sketch. fillet thoes four lines to create a box. Turn that box into a tab. now add a flange to that tab. then edit that flange and include the plane that has not been used (oposit of the origional sketch). use that included line to replace the far edge of the new flange sketch.
I hope to have time to add a vid about this soon.
you end up with an L shaped piece of sheet metal that can be resized every way by only moving the origional planes. The drafted flat pattern can now be created and automatically updated as the design changes.
The reason I bring all this up is whin this context, and adjustible sheet metal part could be very useful.
Adjustable parts are designed for those parts that deform in the assembly -- like a spring. The spring has a single part number but can appear in different deformation levels in all sorts of different assemblies. This is NOT what you want for the job you are doing.
What you are doing is more like a family of parts. Or, if you don't know apriori how the part will change, just have a "seed" part and then when you use it in an assembly and need a different size, use the "Replace Part with Copy" command, which will make a copy of the seed part and then you can modify it all all you like for the new purpose and of course the new copy will get a new part #(filename) because its a different SKU.
PS> I think there are much easier ways to create a parametric box than you are doing, but will let others comment on that.
I am curious about the benefits of or need for assembly planes to adjust a sheet metal file. I would guess that you want to easily change the sheet metal file while in the parent assembly. And, you want to do it with Ordered featuers. Is that correct?
If I understand your desired intent, I would create a contour flange in sheet metal. Draw two end point connected lines in the profile, and dimension them. For example: one horizontal from the origin, and one vertical from the origin. Define the extent of the flange, and SE will automatically put a dimension on it. I would normally use symetric extent, but do whatever your intent requires. Put this in an assembly.
You can use Ctrl+Space to toggle the assembly Select command from part priority to face priority. With ST6 (not sure about ST5) selecting the face of a sheet metal part in the assembly you can Dynamic Edit the component's feature. With the conour flange I described, you would see the height, width, and length dimensions.
In older versions, you can use the Peer Variables to adjust components. You can rename the variables for Height, Width, and Length to make them easily identifiable.
Am I missing some benefit from the assembly planes?
The parimetric box is exatly what I want and have at this point. However this requies all of the perametric parts to be created within context of the assembly and can not be re-used in any other assembly. I have not found any other method of a "perametric part"
My question is: Is there any way to make a perametric part that automatically resizes based upon mate relationship. I want the part to grow or shrink to satisfy how it it mated into position. I will two more twists on this. I want to use the same part in multiple assemblies where it will be a different size in each assembly. And I want it to be adjustable in 3 or more directions.
Simple example. I have a sheet metal flat bar with a hole on each end. I insert the part and mate the holes. I want the bar to become longer or shorter based on the holes it is mated too.
Yes. this is the PERFECT example for Synchronous.
1. Draw up your model. Don't worry about special planes and all that. Just model it (in Synchronous, or move it to Synchronous).
2. Whenever you want to use "some variant" of this model, you place it in the ASM and immediately use the Replace with Copy command.
3. Give it a new filename.
4. Using either the steering wheel or commands like "Make Coplanar" you stretch to fit.
I would encourage you to get more familiar with Synchronous, but doing some of the exercises that the online edumedia provides. And also look up the "Replace with Copy" command.
This video is very similar to what was mentioned by Dan. I'm using here coplanar relate to resize body in the first step. This is in part environment but you can use it in assy too.
Solid Edge offers 2-4 ways (in general) to do what you need.
But you can use fully sketch based modeling method in assy... An other way (I suggest try out synch modeling).
My opinion is that synch is more flexible than "old" history based modeling method.
If you have a exact example I can share my experiences.
I sure wish I would have found that video months ago when I was building some structural steel duct work. I knew that this product was going to have many design iterations and was learning SE ST6 (after several decades of UG/NX). I was looking for the top down design functions and here they are! Thank you, so much for taking the time to educate the userbase!