Family Tables Creating Drawings

[zrehlander]

Hi all,

I have figured out (at least for what I need) family tables and making models from them. I type in either the family table through Pro E or I open the Excel sheet and do major updates. When I go to open the parent model I get to choose which instance I want and it will automatically create the model. This is pretty much what I want to happen but with drawings rather than models. Is there a way to type in the family table and get a drawing to come out automatically just like it does for a model? Using Pro E 4.0 

Thanks,

Zach

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[BenLoosli]

Normally any family table drawing is done in a single drawing using variables for the dimensions that are changed for each instance.

If I have a family table for rectangular plates, I would create a drawing and just use a "Length" and "Width" as the 'dimensions'.

I would then put a table on the drawing with 3 columns - Part Number, Length and Width. Populate the table with the corresponding values and be done with it.

One drawing showing all of the instances and their sizes.

[huggre · Accepted solution]

Hi, here is a short description on haow we solve this issue in my company:

1. Create the generic part/assembly including all its required instances.

2. Create a drawing for the generic part/assembly with all the required views, dimensions etc.

3. Save a copy of the generic drawing

4. Open the new drawing copy and the replace the active model (generic) with one of the instances (and regenreate the drawing)

5. Performe these steps for all the instances in the family table.

[zrehlander]

Thank you. That is where I am at now with the making one drawing and then replacing the model for a new one.

Ben, i have looked into this but we have around 20,000 part numbers so that would get a little hectic on the drawing.

Both were great suggestions though and I can see how that would be very nice to use if we just didn't have so many part numbers.

[BenLoosli]

I hope you don't have 20,000 parts in a single family table!!!

[zrehlander]

no lol.

We do gears and pulleys so I have them arranged by tooth profile for each master shape. So I've got four folders with our master shapes and then I made a part for each tooth profile in each of those four folders and added the family table to every one of the tooth profiles in each folder. So it is broken down a little bit but while were on the subject, how many instances can a family table handle? Because if we use this process long term it could build up in each profile over time.

[BenLoosli]

I was curious and asked PTC what the family table size limitation was and this is their response:

There is no such known limitation on the number of family table
instances. However there is a limitation that depends on the size of the .idx
file which is created after adding the instances. For a 64-bit platform system
it is about approximately 512 000 bytes and for a 32-bit system it's

approximately 256 000 bytes. The .idx files exceeding the size limitation will

not allow to display instances list.

[zrehlander]

Sweet. Thank You!