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pipeline parameters

SOLVED
Regular Member

pipeline parameters

in a previous post this was answered

http://communities.ptc.com/message/175495

and should be similar to this question.

i am trying to write a relation in my pipe assembly to make a datum point the same distance as the length of the pipe.

d19=asm_mbr_pipe_line_len_center:FID_64

maybe only the linestock parameters can be used?

1 ACCEPTED SOLUTION

Accepted Solutions

Re: pipeline parameters

Hi Rusty...

You're attempting to use Pro/REPORT parameters (the "asm.mbr" thing) in a relation. You can't do this. I see you're using the underscores in place of dots, too. That's the nomenclature used when you're writing table relations. But in table relations, you're unable to access dimension values. The good news is, there's a better way!

If you're using the Creo (or Pro/E) Piping module, once you've made your pipe solid, it becomes a standalone part. This part has two pre-defined length parameters you can use in relations: length_center and length_pre_cut. You could then say d19 = length_center:cid_64 (where 64 would be the Component Id of the pipe part). If you don't know the component ID of a component in an assembly you can select Info->Component and pick the component. You're looking for the number that says "Internal Component ID" . You can also get this information by turning on FEAT ID in the model tree. Although it says "FEAT ID", for any components or assemblies, it will list their component ID instead.

Notice the "cid" addition to the relation. This is critical.

This should solve your problem. If you have any trouble, please let me know. I'm happy to help any way I can.

Take care and good luck!

-Brian

View solution in original post

4 REPLIES 4

Re: pipeline parameters

Hi Rusty...

You're attempting to use Pro/REPORT parameters (the "asm.mbr" thing) in a relation. You can't do this. I see you're using the underscores in place of dots, too. That's the nomenclature used when you're writing table relations. But in table relations, you're unable to access dimension values. The good news is, there's a better way!

If you're using the Creo (or Pro/E) Piping module, once you've made your pipe solid, it becomes a standalone part. This part has two pre-defined length parameters you can use in relations: length_center and length_pre_cut. You could then say d19 = length_center:cid_64 (where 64 would be the Component Id of the pipe part). If you don't know the component ID of a component in an assembly you can select Info->Component and pick the component. You're looking for the number that says "Internal Component ID" . You can also get this information by turning on FEAT ID in the model tree. Although it says "FEAT ID", for any components or assemblies, it will list their component ID instead.

Notice the "cid" addition to the relation. This is critical.

This should solve your problem. If you have any trouble, please let me know. I'm happy to help any way I can.

Take care and good luck!

-Brian

View solution in original post

Highlighted

Re: pipeline parameters

Brian,

I was reading your response to the question about piping parameters and Pro/Report Parameters.
I was curious if you've ever had to deal with detailing the tube solid separate from the assembly.
At my company we define our tubing assemblies and detail each of the parts as a separate drawing for tracking and manufacturing control purposes. The problem we have always had is getting a bend table that displays the bend locations of the tube. You can do this at the assembly level by designating a report for the Bend Location and using the parameters "&asm.mbr.pipe.segment.csys.bend.loc_" in a table. But you can't do that for the tube by itself. Is there any way that you know of, of getting that information into the tube or linked in some way?

Thanks,

Corey

Re: pipeline parameters

Hi Corey...

Yes, I've had to deal with this before. To get the bend table, you need the assembly (as you've already mentioned). So then, go ahead and make a drawing of your part. Then, add the assembly as a second model to your drawing. You don't even need to display any views of the assembly... just load it as a model and use it to get the bend table.

You can filter the bend table results to show only the bend information for one specific pipe. When you're done, you'll have a drawing with views showing one individual pipe. You'll also have a bend table showing only the information for that one specific pipe. The only downside is that the assembly is actually linked to the drawing, too. In many cases this isn't a problem. If it is... there are some other ways you could get around the problem.

One thing you could try would be to make a drawing of each individual pipe/tube... and then publish the bend tables as a separate document. All of the bend tables could be generated from the assembly and stored in this separate document (a Word document, Excel spreadsheet, etc). Then, on the field of your individual drawings you could reference the bend table in a drawing note. For example: "1. Manufacturing information for this item is contained within Document #123."

Another approach might be to change the way each pipe/tube is detailed. Instead of loading the individual solid pipes into a drawing, maybe you could simply load the assembly instead. Right now you load the individual solid pipe and then have trouble creating the bend table. Instead, load the assembly into the drawing and use a simplified rep to show only the individual pipe you're interested in. You can then show the bend table easily (because you're using the assembly). Then you could filter the bend table to remove all information from the table except the data for the pipe you're interested in. This makes it look like you've created a part detail, but really it's just a specialized assembly drawing.

Would there be any objections to loading the assembly into each part drawing just so it can drive the bend table? If so, would your company go for the idea of publishing the bend tables as a separate reference document? If none of those ideas works... maybe you could open the assembly model and save the data from the bend tables into a separate file then link that file to the individual pipe. There are a couple of ways you could do this. You could store the table as secondary content in Windchill and attach it to the drawing. Or, you could store the table and link to it using a note and URL hyperlink in the drawing. Or... better yet, maybe you just could just copy the table into the field of the drawing itself. The downside to this technique is that the table will no longer dynamically update as the assembly changes.

I realize that none of these solutions are giving you the answer you were hoping for. But as far as I know (unless something has changed in Creo 2), there's no way to access that bend table information at the individual solid pipe level. Maybe this will change (or maybe it already has). I haven't used the Piping module in Creo 2 yet. In the absence of some grand change that suddenly makes the bend table information available in Creo 2, the techniques above are your best bet.

If you need more information or help implementing any of these options, write back and I'll do my best to help.

Thanks!

-Brian

Re: pipeline parameters

Brian,

Thanks so much for the detailed and very concise response. Much appreciated!

So I summarized the options here:

1) Add Assembly as hidden model to drive bend table

2) Bend Tables released as separate document

3) Use assembly in simplifed rep mode to display individual tube

4) Separate bend data into another file then link to drawing of tube

We've used options 1 and 3 on various occasions.

For options 2 and 4 I can ask different programs if they might consider that, but it defiinitely would be out of the norm of what we process now.

I've looked into Creo 2 and the piping module now does send some data to the solid tube part via parameters, but only things like wall thickess, OD, material, length... Nothing in regards to the bend information, which is shocking since they took the time to send the other data over, but not the data that actually defines the tube completely.

Another option we've done is we build the top assembly where each tube is its own sub assembly which gives us an extra model with the same name just two different extensions (i.e. asm and prt) And it stays linked up. It's a bit hokey, but ends up giving us flexiblity to control the release process of each tube.

The options of 1 and 3 have the down fall of the assembly going along for the ride. Sometimes with programs with short schedule runs we'll release things early like the detail parts and get the assembly out later. With 1 and 3 the assembly would have to release with the details. Most of the time this isn't a problem since most line assemblies we have are simple one tube and two flanges. Unfortunately new programs are coming up with much more elaborate tubing assemblies that this option won't work very well for them.

I have a case setup with PTC asking why they took the time with Creo 2 to send some data to the pipe solid, but not the most important data required. Maybe they'll give me a magic bullet that gives what we'd need, but I doubt it. I'll let you know.

Thanks for your insight and time!

Corey

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