How to add driven dimension into the family table

I'm creating a family of sheet metal parts. Simple bending only. I'd
like to add dimension of unbend (flat) part into the family table. I'm
able to add needed dimension into the unbend (flat) part in drawing
mode, but I can't add it into the family table.
Have you got any idea?
Thanks in advance.
Wojtek
WF1
Reply to
Wojtek Weber
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I can think of two ways you could make a parameter that you could include in the table and whose value you could use in a repeat region. But in both cases they'd be derivative, measures, calculated values and wouldn't control anything. So the purpose of putting such in a table is a little obscure. You could certainly create these parameters and use their values in a table or drawing without putting them in family table.
* Create a parameter ('Tools>Relations') by assigning it the sum of the values of all the features which produce the length, e.g., t_length=d5+d8+d10. This will work if these feature dimension variables remain the same within an acutal family of parts. * Create a measure feature ('Insert>Model datum>Evaluate') and use this to create a parameter containing/recording this value.
David Janes
Reply to
David Janes
Wojtek, did you add the feature of the unbend into the table? We us the Flat State command under the sheet metal menu manager to creat our flat states and it work really well. Your also trying to add driven parameter right and not a created one? If the parameter is i the drawing only, then you can not add it into the family table
Hope this helps, Glenn |B
Reply to
GWDavis28
Thanks for answer. The reason I need additional dimension of the flat part is very simple. Quality department needs documentation containing this dimension. So I'm adding it into the simple drawing of a flat part (flat state). But I'm not able to create the table containing this dimension (or better dimensions) in the family of the parts. Of course it is possible to create parameter as you've described. This is known feature. Anyway for more than two bends it produces formulas which are very complex and difficult to maintain. So I've started to search the easier solution.
The second solution is unknown for me. I haven't got `Evaluate` under 'Insert>Model datum>` menus. I'm using WF1
Wojtek
Reply to
Wojtek
Thanks for answer. The reason I need additional dimension of the flat part is very simple. Quality department needs documentation containing this dimension. So I'm adding it into the simple drawing of a flat part (flat state). But I'm not able to create the table containing this dimension (or better dimensions) in the family of the parts. Of course it is possible to create parameter as you've described. This is known feature. Anyway for more than two bends it produces formulas which are very complex and difficult to maintain. So I've started to search the easier solution.
The second solution is unknown for me. I haven't got `Evaluate` under 'Insert>Model datum>` menus. I'm using WF1
Wojtek
Reply to
Wojtek
Thanks for explanation. It makes me sure I'm doing all the work correctly, but I don't know some tips and tricks (if they exist).
I'm using Flat State command and later create two model drawing. It means there is a complete, bent detail and Flat State on it. Standard dimensions shown on the drawing (view) of the flat state are not acceptable to me. So now I'm simply adding needed dimensions and hiding the other ones. Of course added dimension do not control anything. But they are important for control purposes during manufacturing. It works OK for one detail. Now I'm creating family of basic i.e. bent details. Flat state for the other details from family are created automatically. And so I'd like to have not only dimension from model, but this added dimension grouped into the table and assigned into the particular family member on the table. I also desire this dimension changes automatically when some changes are introduced into the generic and/or the family table.
Hope it's understandable. Anyway, I'm afraid this feature is only desire. Am I right? Or any simple solution exist?
Wojtek
GWDavis28 wrote:
Reply to
Wojtek
You can test out the following technique to see if it provides you with what you're looking for here.
1) Retrieve the flat state instance and add Part mode Reference Dimensions to it. In Wildfire you can create Part or Assembly mode Reference Dimensions two different ways. The first way is to choose Edit - Set Up - Ref Dim. You will have to select a datum plane for the dimensions to be parallel to. The second way is to add what is known as an Annotation feature Ref Dim in Wildfire 1 or 2. There's an icon on your Wildfire toolbar for Annotations. This approach also requires the user to select a datum plane for their Ref Dim to be parallel to. After you have created the first Ref Dim you can then select this Ref Dim to orient the part for subsequent Ref Dims' creation. Once you have your Ref Dims created, perform a Switch Symbols operation so that you can see the Ref Dims' Symbol Names. Such as rd0 and rd1, as examples only. You can also do this by choosing Tools - Relations.
2) Retrieve the generic model and choose Tools - Family Table. Click on the icon for adding dimensions, features, etc. and choose the option named 'Other'. Pro/ENGINEER will prompt you to enter a Symbol Name. This is where you can enter the rd0 and rd1 or whatever your Ref Dims Symbol Names turn out to be after having created them in the flat state instance.
This should solve your problem. You can also use the 'Other' option to include dimension tolerances in a Family Table. Not that there is much of a demand for this type of thing, but I thought that I would offer that up to you while I am discussing the 'Other' option in Family Tables.
Ron M.
Reply to
Ron M.
Wojtek, :( Sorry man yah this is not possible. Created dimension (dimensions added into a drawing) can not be used in a family tabl to drive/change models.
As an alternative, you could always create your parts in the flattene
state get the driven dimensions you are looking for and then add thos to the family table
I guess it all depends on what's most important to you. Th
parameters/driven dimensions or the flattened state or the forme state
You could with some work create the family in the flat state and hav
all of the driven dimensions for both states so that they can appea in the table. But you'd have to look at the parts and determine wha can be made commonly. Though it's easy for me to talk since I don' know what your parts look like
Anyway, good luck and let me know if I can help with anything else
Later, Glenn |B
Reply to
GWDavis28
Thanks a lot for the information. It works, but not solves the main problem. I've checked it doesn't work because Flat State became part of a family table. You can add ref dimension into the family name, but they are not updated when model is changed. Anyway all the information I've received from you and from other guys is extremely useful to try to solve the main problem by myself. Seems ProE do not allow to create really useful family table for Flat State in simple way. The only way is to create some parameters and relations.
Wojtek
R>
Reply to
Wojtek Weber
Thanks a lot for the information. It works, but not solves the main problem. I've checked it doesn't work because Flat State became part of a family table. You can add ref dimension into the family name, but they are not updated when model is changed. Anyway all the information I've received from you and from other guys is extremely useful to try to solve the main problem by myself. Seems ProE do not allow to create really useful family table for Flat State in simple way. The only way is to create some parameters and relations.
Wojtek
R>
Reply to
Wojtek

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