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# sheet metal part views

#### tomh

##### New member
How can I show both bent as well as flattened views of a sheet metal part in a drawing?

Thanks,

Tom

Family table - flat & bent instance, add both models to the drawing.

Thanks dr_gallup. I'm doing that already, but I find this method obtuse. I was hoping that there was a command or option to account for the obvious fact that both the flattened state as well as the formed shape need to be detailed.

Thanks

I think that PTC was thinking about renaming PRO/DETAIL to PRO/"We've spent a lot of time and money on the modeling and had a crew of chimpanzees design our detailing"

I just spend 15 minutes learning how to dimension a bolt circle and 30 seconds doing it. It should have taken 5.

I also ran into the seemingly intuitive need for sheet metal (flat and bent). It is fairly easy to do, but it seems like a silly implentation.

I strongly feel that you should be able to represent a flattened view as well as a formed/bent view of a single sheet metal part. Now I am forced to create additional parts to represent one single part. Where is the logic in that?

I think it is very logical, they are not the same part. I frequently need to have various states of "bent" such as a flat terminal that gets insert molded into a bobbin. Then the coil is wound and one leg of the terminal is bent. Then the coil assembly is put into an upper level assembly and another leg is bent. The functionality is very powerful.

Use edit-> setup -> flatstate bam you got your flat.

dr_gallup,

What you explain is various states of a part as it lives through manufacturing an assembly. It's perfectly logical to consider these different states being different parts living inside a family table.

The case Tomh is referring to is a "simple" sheetmetal part that needs manufacturing. By the sheer meaning of the word sheetmetal the part has a first manufacturing state where it is flat, cut out of sheet and a final state where it is bent into the form it needs to have to be functional. We're only intrested in the first and the final state, and even then the flat state is only necessary to communicate what has to be cut and as a check for the designer that no impossible overlaps exist. Although the sheet can have 50 partially bent states in between cutting and finishing, that's only of intrest on the shopfloor, not for the designer.

The flattened state is, as it says, a state of the part. It is not a part as such. So it sounds logical to metoo that it would be considered as such. Whenever retrieving the part you should only see it formed as intended. Only in detailing you should be able to set a view to flattened state or formed state.

My 0.02 Euro

Alex

pmack009,

I know about the flattend state (Create Flat Pattern in WF2.0), but that does not give me the option of showing both the flattened and the bent part in the drawing without suppressing the Flat Pattern feature, which then disrupts the views that were displaying the part (including all dimensions and call outs) in its bent form.

Thanks though,

Tom

I spoke with PTC today and they told me the only option was to create flattened instances of the formed parts....

Thanks for the input though.

Tom

Yes. I would like to show a flattened view as wells as the bent view of one part on one drawing sheet.

ON WF2 you just right on the screen and pick drwing models add pick the base number of the part and pick the flat family table value

Tomh - you could probably make a mapkey that would automatically make a flatened instance of your part and put a view in your drawing. I'm not sure it would be worth the effort. My point is that with family tables you can do so much more than just have a flattened sheetmetal part. It is extremely useful and productive for all kinds of modeling so you should get familiar with it.

Mapkey to make the flat. No I don't think that would work. you need to pick a surface. But may be you can pause the mappper for this?

Yes if you want to get good at Pro-E you will need to know the Family tables. you can do a lot with them. and with complex sheetmetal parts it's a must.

I have done something like this:

Open the part and add flat pattern feature..

Create one Family table with flat pattern feature as table item

for Generic part set:Yes

for Instance set:No (i.e it will suppress the flat pattern feature)

use the required instace in DWG..

I hope this will help U..

Edited by: dineshkumarjkk

Another way of creating a flat part is to create an instance (call it part_name-flat), open it & create the flattened part in the instance and save.

The original model now has the end result, while the instance has the flattened outline.