alternative to simplified rep in Pro/E? 2

[gross]

Hello Eng-Tip Members.

I have a pro/e question. First my situation. I'm using a flex hose in my assembly twice but each hoes is bent different. I do not want to start a simplified rep ripple in my assemblies.

Is there a way to have 2 different parts (because of the way they are bent in the assembly) to be called up on the BOM as a qty of 2?

thanks for reading

 

[442olds]

Yes there is an alternative. You can set up variable geometry parts. basically you name the part part_name_vgxx.prt or .asm where xx is 01, 02,...and on and on.

Then I don't know how its done because the table parameters are already setup and I'm pretty new to the Pro/E game, but I would imagine that you will need to setup the repeat region to read only the first part of the part name (ie the part number) that you want to show up as qty 2, 3,... or however many you have. It will probably take some trial and error part on your end, I personally have not had to attempt to make the table yet.

 

[gross]

I have set up relations in my table to read the different parts as the same name but the table creates a seperate line for each part. I would like to combine different parts into one line.

thanks for your comment.
Caper

 

[atlarson]

One method that will allow you to have multiple models combined into one line in your parts list is to create a parameter in your parts and assemblies called &quot;part_number&quot; and then replace the entry &quot;asm.mbr.name&quot; in your parts list repeat region with &quot;asm.mbr.part_number&quot;. This is done (in version 20) by selecting <table> <repeat region> <switch syms> <done/return> <modify> <text> and selecting the cell where the part name is found.

If you decide to use this method, it also helps to create another repeat region outside of the drawing border that contains both &quot;asm.mbr.name&quot; and &quot;asm.mbr.part_number&quot;. This will allow you to add the &quot;part_number&quot; parameter to all components while working in the drawing model by entering information into the table, instead of creating the parameters in the part or assembly models. This extra table can be deleted or layered off before the drawing is released.

 

[Hora]

Hi Gross,

There are several methods to do that.

FIRST METHOD is like ATLARSON said to create a pararameter in each part and drive the BOM TABLE with the parameter &asm.mbr.part_number or whathever. But the main incovenient is that if you realized at the end of your project you need to use this parameter, you must assign this parameter to all your parts from assembly, or to modify you format table (create another repeat region able to use this parameter assigned on part in question only)

THE SECOND METHOD is to create a parameter let's say &quot;qty&quot; (derived from quantity) and to use it in your table region. The qty must be created in drawing mode. The advantage of using this method is that you modify only the BOM table of the specified drawing only and not the parts or assemblies. You can use this parameter in this way:
Choose TABLE -> REPEAT REGION -> RELATIONS -> click on your BOM -> EDIT ->

IF asm_mbr_name == &quot;your part name here&quot;
qty == 2 (or quantity you need to see)
else
qty = rpt_qty
endif

In this way you can control the quantity of items in your BOM.

IMPORTANT: Now, your table will show both parts (one with qty of 2 and the other with a qty of 1). But you don't need the second one. You will need to exclude from the table:

TABLE -> REPEAT REGION -> FILTERS -> click on table -> BY ITEM -> EXCLUDE -> click on the part you want to exclude.

THIRD METHOD:
Go to ASSEMBLY mode, and choose: COMPONENT -> ADV UTILS -> INCLUDE -> choose your part that you want to be in a qty of 2. Now the part will be part of you assemby, but you are not able to see it.

Go back to your drawing mode and regenarate the drawing. You will see a qty of 2 for the part in question. It will rest only to exclude the second part from the table (see method 2). That's all. It's fast, clean and works well.



Good luck!