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Funny you answered I was just looking at the posting on layers.
Okay about the paramers in a bom. I AM able to put the parameters in a free standing note, and it updates as it is supposed to, HOWEVER, when i add the notes to a bom, NO-GO it just stays in the '&d0' format.
BTW what does even essential mean?
BTWBTW- i have tried to search the bohemoth that is the mastering layers posting but I begin to nod off before i find what i am lookin for so i'll ask you. How do you use the search function to add items to a layer Edited by: jelston
Once the table is setup and the repeat regions established, double click on the cell, and a menu will appear. Make the picks asm> member> user_defined> and enter the model parameter name desired. When complete the repeat region text should be something like asm.mbr.descripton or asm.mbr.part_number.
Layers from the find dialog:
Get the Find dialog setup so it lists the items desired, then choose Options>Save Query>name the layer.
Second, is there a way to enter the type of information via the model tree? I ask this because entering the information in a cell, binds that cell tothat information only, which would be find if all my parts are exactly the same. If it can be entered individually in the model tree then i can customize each entry.
you can add the particular parameter as a column in your model tree and then edit that parameter for that part. You can also highlight multiple parts in your model tree which you want the same value. Like a material parameter for instance you could highlight every component in your model tree that should be aluminum and then RMB->edit parameters input aluminum for the material value and now all those components have been changed.
Second, is there a way to enter the type of information via the model tree? I ask this because entering the information in a cell, binds that cell tothat information only, which would be find if all my parts are exactly the same. If it can be entered individually in the model tree then i can customize each entry.
I'm not sure what you mean about the entering of information in a cell being bound to that cell.
In a drawing table, one setup for use as a bom, the table is defined to have a repeat region, then cells from the repete region are filled with very specific syntax. Once setup and depending on other repeat region settings, the table will expand automatically, one line for each item in the assembly. And each cell will be automatically filled in with the relevant model parameter. The values shown can be selected and edited, causing the model's parameter to be modified. The exception being if the model has no parameter for that column. What does not show can't be picked.
Repeat regions can only carry items that exist in all the models. I've not done it in a bom, but it should be possible to include dims of each model. The trick is that the relevant dimension in every model must have the same symbol name.
The dimensions have a reference back to each model. For d1:92 may be dimension 1 in model 92 (something like that). But I don't think it is possible. I miss SW.
Here is a solution for you to try. Create a generic part for the sheetmetal part, fitting, bolt (3 parts). Create a family table for each part with the dimensions you want to change. In the parameters list of the generic instance for each part create parameter values you want to use in the BOM repeat region (DIA, LENGTH, etc. for the bolt). Create a relation in the generic instance for each part that sets your parameter value equal to the dimension value (DIA=d3, LENGTH=d4, etc). Verify the instances in the family table. In the drawing table set one column with the &asm.mbr.name (selection is asm>mbr>name). Set the second column to &asm.mbr.DIA (selection is asm>mbr>USER_DEFINED, it will ask you for parameter name). You can combine the parameters or place them in a different column. When you replace a part, the bolt for example, with another part in the part's family table, the DIA, LENGTH, etc. will automatically update in the drawing table.
Is there a good reference for what the report sysmbolsgive you or is this just a matter going through each parameter and making a note on what it does? For instance, I have gone one level deeper into the report menu, chosen what I thought was the value I wanted, and it returned a value that I wasn't expecting.I tried the method you show in the pdf. The problem I had was, if you had say three report symbols in one cell and you use a model that didn't have one of those symbols, the & symbol would be stripped from the report symbol that was missing and the parameter name was left in the description (name DIA LENGTH: bolt .750 2.00: plate DIA 14.00).
<div style="margin-left: 40px;">The problem I had was, if you had say three report symbols in one cell
and you use a model that didn't have one of those symbols, the &
symbol would be stripped from the report symbol that was missing and
the parameter name was left in the description (name DIA LENGTH: bolt
.750 2.00: plate DIA 14.00).
</div>I don't think I understand the problem as stated.
In my example, neither desc or length existed in any of the models, until after the drawing and the table were created. The table showed empty and as the desc was added to each part and as the dim symbols were altered to "length", it filled in.
BTW the bottom row of that table is not part of the repeat region. The notations there are to show what symbols were entered into the next line up, where the repeat region was defined. Hope that didn't through any one off.
Sorry for any confusion. I mixed up some of the results I was geting.
I think my problem was the drawing format I was using didn't have a BOM table with a repeat region as it should have, just a plain table. To put my question in a context, I have an assembly that contains plate and bolts. My BOM table has a DESCRIPTION column and usesone repeat region.When the BOM table is updated for the assembly the bolts and plates are in therepeat region. For theDESCRIPTION of the bolts I want to show the NAME, DIA, and LENGTH of the bolt. For the plate I only want to show theNAME and LENGTH. From my understanding of repeat regions, because I have one repeat region and parts that have a different number of parameters for the description, I need to include all the parameters in the DESCRIPTION columns first cell. So I end up with a cell that has: &asm.mdr.NAME, &asm.mbr.DIA, &asm.mbr.LENGTH.
My question is, for the plate, will the repeat region return just the NAME and LENGTH? The first time I tried this for the plate, the cell returned plate, &asm.mbr.DIA, 14.00. For the bolt it returned all the values bolt, .750, 2.00.
As far as the part about stripping the & symbol from the report symbol, I was trying to input the parameters manually to see what would happen: &NAME:2 &DIA:2, &LENGTH:2 (for the bolt). The number I input found a plate and returned plate, DIA, 14.00. I found out that the number after the DIA parameter was not the same as the other two and for the plate should be removed. The result was plate DIA:4 14.00, which indicates that there is no part with that number. Is there a way to find out what numbers are assigned to a part or assembly without trial and error (changing the number until you find one associated with a part)?
It would be great if Pro/E had a bit more functionality in relations. Specifically it has no function to convert a real number directly into a text string. Or maybe just enable something called data coercion.
To be able to write a model relation that says, description="BOLT"+&D1+"DIA " would be so useful.
As it is, the easy way out is to simply edit the description to include
what ever is needed. It's not parametric everyone spends way too much time filling in a bunch of boxes, and the checker has to be
extra careful. This actually works for things like fasteners, as you only have the get it right once.
I
have used RND to round up the last decimal place, what it is doing is
using the "floor" function to truncate the number, then subtract the
truncated number from the original to get the decimal part. This is
then multiplied by 10e2 to give the right number for 2 decimal places
In the text output (TITLE_1) you simply add the truncated text part to the decimal text part and job done.
You can apply a similar method to other values to get more information into the text string as required.
Yes, that works. But it doesn't pass the easy to use test. As things are it's easier to just modify the relevant text that to mess with that set of relations.
I see a conversion from mm to inches in that set of relations.
Have you considered specifying the units of the parameter instead of hard coding the conversion. By defining x_inch to be inches and x to be mm, proe will handle the conversion automatically. Whats more, the relation will be bulletproof against someone changing the units of the model.
I was merely describing a method of getting a decimal number (decimalised imperial in this case) to show AUTOMATICALLY in an ITOS, far easier than editing the parameters for every part especially when family tables are involved (I only use this in family tables).
We model our parts only in mm, when including a decimal in the description this method is used whether it be for an imperial conversion or otherwise. We export BOMs easily and it works for us.
The setup is easy to use if you know whats going on. Just cut and paste the text and change the names of the relevant dimensions.
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