Help- model_name or Drawing_name

[dcharles]

Bit of a mix up here. I have an assembly which is updated via inputs from a layout table. Depending on the values entered in creats a new model for certain components, and chooses a suitable component from a family table. In simple form, it designs a new bolt, yet chooses a family table driven nut based on the thread. However, my assembly drives two drawings (both sepeate drawing numbers).

The problem is:-

On the drawing sheet, if I choose the drawing number as DRAWING_NAME it brings up the dawing name ok (ie drawing file name), but if I was to use a Family Table component for a detail (each instance has it's own part number). The drawing number would be the GENERIC Model not the individual part number as shown on the Family Table. I can get round this by assigning my drawing number as MODEL_NAME but as I produce 2 Drawings from my assembly, it only brings up the assembly name (I need 2 differing drawing numbers). How can I get round this as I only want 1 drawing format and obviously running Intralink, it would make it easier to search. Does this make sense?

Please help.

 

[onlyadrafter]

Hello,

Can you clarify a couple of points. As I understand it, you are doing the following.

1) Regenerating an assembly.
2) A new size of bolt is created, from certain inputs.
3) A nut is chosen from a family table, depending on the size of the bolt.
4) You are creating two drawings. (OF WHAT, COMPONENTS OR ASSEMBLY, OR ONE OF EACH?)
5) You want the component/assembly name in the drawing title box.

As a quick guess, if you are creating a drawing of a component, when you SET MODEL to the component, edit the &model_name (which will be something like &model_name:2), remove the :2 and hit OK, will this not change it to the model name of the component. If this is way of the mark please clear up numbers 4 and 5 from above.





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Hope this helps.
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maybe only a drafter
but the best user at this company!

 

[dcharles]

From the assembly I am creating 2 different and seperate drawings (for simplicity, one showing the assembly, the other showing some tensioning gear). We have two have seperate assembly drawings because of the way we work. However, as we only want one drawing format, we want to know what we have to put in the box where the drawing number should sit. I can undersand that if I put &model_name, it will display the model name (i.e. if the model is called by the part number), and if I put &dwg_name, then whatever the drawing file name is called then that would be it.
The problems arise when we use that format for a family table component. As if we use &model_name, it works (but we cannot use that format for the two assemblies as it runs from the same model). If we use &dwg_name it doesn't work as if we replace the component in Views menu on the drawing module, it shows up as whatever the generic model is called, not the family table member name.

It is important we get this right, as we will be using this through Intralink.

Is this any clearer?

We are running 2001 PROE.

 

[im4cad]

Please correct me if I'm wrong, but I think that you can create as many drawings from the same family table, using as many instances you want, but the drawings will bear the generic's name. You can keep one of them with the generic name, and manually change the names for the others. If there's another way to do it, I'll be glad to find out about it.

im4cad
Pro Design Services, Inc.

http://www.cadproe.com/pds/home.asp

 

[onlyadrafter]

Hello,

Could you not create a parameter for each part and instance called 'real_name' for example, you could then put this is the Drawing Number box.

Is this suitable?



----------------------------------
Hope this helps.
----------------------------------

maybe only a drafter
but the best user at this company!

 

[bigroy]

Hi,

Complete entirely your the most complex of your two drawings. I suggest you use drawing name as your title block driving field. Once you have completed this drawing you can save as to the next number you require. When you open this drawing you will be able to replace the model with one of your family table members.

You can work with multiple models in your drawings. You will need to add the model to the drawing and set the required current model if you switch between them. I use this when I need to show assemblies in location on other assemblies some of the models are for convenience only and you don't want them appearing in your BOM for example.

If you need views of the generic you can use it. If you want details or smaller assemblies you can add them also. Remember though that if you use a driven BOM this will refer to the current model at the time the bom chart or format is added.

If you really want you could use a multi sheet drawing (single filename), and add "sheet &sheet of &total_sheets" to your format. This would differentiate the different pages.

I hope this helps.