Drawing table with profile lengths (flexible component)

[KB_11240762]

Hello,

I'm using Creo Parametric 10.0 and I have a quesiton.

Is it possible to have table on the drawing with lengths of each profile?

Example how I want this table to look like:
2 PCS | Profile 50x30x2 | 250 mm

3 PCS | Profile 30x30x2 | 150 mm

1 PCS  | Profile 30x30x2 | 120 mm

I've created generic profile model with instances and I'm changing lenght of it by "making it flexible".

I want to have this "flexible" length in table.

Is it possible? 

Thank you all for your help.

[kdirth]

I don't believe this is possible.  Flexibility does not change the part/subassembly file.

What you need to use is Family Table.  This creates one part with many versions.

[kdirth]

Here is an example part with family table for the 3 example variations.

[Van_AG]

In the family table of profile.prt add a variable parameter (for example, ptc_common_name as the profile name) and a variable dimension (for example, d4 as the profile length).

See pic1.

In the drawing

Create a 1 row/3 column table.

Create a repeat region with type "Simple" for all three cells.

Set attribute "No Duplicates" for the repeat region.

Type in cells

1st: &rpt.qty PCS

2nd: &asm.mbr.ptc_common_name

3rd: &asm.mbr.d4 mm

See pic2 (symbol "&" not displayed but exist in cells).
And for result see pic3.

---

It is strange to use both the family table and component flexibility in your case,
Use a family table if each component must be a separate BOM item.
Use flexibility if the same component has different geometry at different locations in the assembly.

For example, if it is a spring or a rubber seal.

[Radovan_DT]

It would work but you would have to manually check out every dimension and write it down in relations which is very time consuming. Its better to use family table as mentioned from other guys as you just do it once there.

[KB_11240762]

Hi,

Thank's for previous replies.

Why I'm using flexibility?

Example:

I want orange profile to have the same length as distance between green profiles.

I don't need to measure anything, just click 2 surfaces and it's done.

For family table and relations i need to create a lot of instances or a lot of relations. I want to avoid it.

I want to use the same instance many times and change just lengths.

So I'll ask again, does anyone has idea how to show this "flexible" length in table on the drawing?

[kdirth]

Have you looked at using Advanced Framework Extension (AFX) for what you are doing?

About Working with Creo Advanced Framework (ptc.com)

[Radovan_DT · Accepted solution]

I tested it once again and managed to do exactly what you want, its suprisingly pretty easy

1, Create relation for length of your profile IN PART not in assembly

2, In the table put in &asm.mbr.delka in new collum (or you can combine everything in first collum like [&asm.mbr.ptc_common_name - &asm.mbr.delka]

3, profit

[KB_11240762]

Hi,

It works! Thank you so much!

[KB_11240762]

One last question.

Can you tell me how to set 0 decimal plases in the table?

[kdirth]

Round Parameter Value:  add [.X] after the parameter name, X being the number of decimals.

example: asm.mbr.d4[.0]

[KB_11240762]

It works, thanks!