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Can I use family table values in my drawings?

gregarpp

New member
How can I add values from the family table to my notes and text?



I can use my parameters by doing &parm_name



is there something similar for family tables?



thanks!
 

Ascorti

New member
In reading your question, it seems to me to be rather vague. What values are you trying to add to notes and text? I do not think you will be able to show family table values in notes and text due to the fact that, using dimensions as an example, that the dimension id is the same for all instances. Please post a reply if you find a way to make this work.
 

Ascorti

New member
In reading your question, it seems to me to be rather vague. What values are you trying to add to notes and text? I do not think you will be able to show family table values in notes and text due to the fact that, using dimensions as an example, that the dimension id is the same for all instances. Please post a reply if you find a way to make this work.
 
1. You need to put instance of the part you want to use the family table value from into the drawing.

Let's say you have 'generic.prt' with instance name 'part1'.

You need put model of 'part1.prt' into the drawing.



2. Find out what session id is of 'part1.prt'.

Easy way of doing this will be, create a view and show a dimension, then switch_dim, this will show dimension as 'd41:5'

Then session id is 5.



3. Create note using '&d41:5' for dimension or '&parameter name:5' for parameter.
 

tham

New member
To add a dim from your family table to the drawing:



(I'm assuming the item in the family table is dimension from a feature)

1. Add the dimension to the family table using the normal method of selecting the dimension.

2. Go back to the part (or you can do this first, it doesn't matter). Assign the dimension a symbol by:

MODIFY > DIM COSMETICS > SYMBOL

(then pick your dim and give it a name).

You will notice the name you just entered will show up in the family table.



3. Then you just insert it into your note like Charles said using & followed by the symbol name you entered (ex... &hole_depth)
 

kvision

Moderator
If the notes are attached to items with leaders then you can also use &param_name:att this will pull the parameter from the current instance which the leader is attached to.
 

skraba

New member
I assume you are trying to add basic dims of the parts to the drawing. If this is not the case, stop reading here.



E.g., you have part (screw) with basic dims (diameter and length). Assign parameters to that part's familiy tab, that is add parameters diameter and length. Then you need to assign value from family tab to those parameters. You can do that by writing the following to the relations section.



diameter=ITOS(d1)

length=ITOS(d2)



where d1 and d2 are dimensions of the part model. ITOS function converts real number or integer to the string, which is needed by drawing parameter. But, to warn you, ITOS function also suppresses trailing scale numbers, so parameter diameter with dimension d1 value of 14.5 will result in value 14, not 14.5.



Parameter to bind with assembly drawing is e.g. measure. So you have to add the following to the relations section:



measure=diameter+x+length



(All of the strings in the equation above have to be String data type.)



To add that parameter to the drawing, simply type &measure into the note's text section.



I hope this does answer your question.
 

francis

New member
O.. Confusing,



I have one rectangular block with varying length .



For this I have made one family table.



And this family table value I need in Drawing with instance name and length.



I think this is the question Mr. gregarpp wants to know
 

amd450

New member
I want join 2 tables (endpoint with endpoint), but I dont got, there are only the option >in entity , in vertex and others, but I dont kwow which I can use.



Andre Almeida
 

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