cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Hoses/pipes with windchill

gfraulini
17-Peridot

Hoses/pipes with windchill

Hi all,

First of all, I talk about pipes/hoses of which I've made the part (file.prt) starting from the "pipe center line".

I see that when you use pipe mode linked with WC, every time you load an assembly with hoses, the program feels that the assembly are changed also if you have not touch anything, also because you have only opened the file.

ProE/WC asks you how proceed: check-out or modify the parts (the hoses).

Which is the right procedure to solve this issue?

Thanks

Bye

14 REPLIES 14

HI, Can I ask how you are making the end references for the pipes/hoses?

I try to do these as measured transforms it stops the assemblies from reading data each time you open if you have created external or circular refs.

If you have circular refs then you will always be looking to read data in and WC will see that as a change.

gfraulini
17-Peridot
(To:rcrerar)

Hi,

I make two coordinate systems into the top assembly and I use those as reference for the in/outlet of the hose. All the references are within the top assembly and I haven't circular references.

Can you share a view of the model tree please?

gfraulini
17-Peridot
(To:rcrerar)

Cattura.JPG

Here it is.

As you can see, each hoses has their constraints within the assembly.

Bye

Thanks for sending that. It is clear to me now.

PM1010D200-PM1097 is the top assembly. You have all mechanical components assembled in below that which is as I would expect.

Your Pipes are directly under that assembly and look fine. The only thing that I suspect is causing the issue is if the co-ordinates are created on another co-ordinate or referenced in the assemblies below. If that is the case then they will be looking to confirm the position each time. check UTENZA_1 and UTENZA_2 for example.


To break that link, if that is the issue, I would measure a transform and use that file to create the co-ordinate system in PM1010D200-PM1097


/analysis/measure/transform click on 'i ' and save out the file. The file can then be used to recreate the co-ordinates UTENZA_1 and UTENZA_2 for example. This will break any relative links to geometry and you will no longer have the check-out/modify message.


You might want to try this on a smaller model first.



gfraulini
17-Peridot
(To:rcrerar)

Thanks

I will try soon and I'll tell to you!

How did you get on with this? Hope it worked out for you.

gfraulini
17-Peridot
(To:rcrerar)

Hi,

unfortunatly It didn't work...in an assembly with many hoses, each of them with the start/end on a cys attached on a component, some of them required the regeneration and the others no.

The assembly attached at the post is an example: two hose, aspirazione_1 and aspirazione_2; if I open the assembly just downloaded from windchill, and so I've not modified it yet, and I do the regeneration, proE feels modified only aspirazione_2 and if I want to save, I have to put in check-out the aspirazione_2 and the top-assembly pm109d00...

Hi,

I am working on creating the machine which will show the Pneumatic and Hydraulic lines from panel to the other units in the machine. How to create hoses in a effective way, it takes lot of time to create one line of hoses since we have to create the route points by extend and then providing the X,Y,Z dimensions and again editing the route is a big pain or we have to create a datum points using offset co ordinate system to select the route points. Is that any other better way to do it by simply dragging the

co-ordinate system to the desired location along the route points. I have to create nearly 40 tube lines which spreads all over the machine.

Appreciate your help

Thanks

The problem is caused from the regeneration for the mass property.

If I only regenerate the model nothing happens. but if I regenerate the model imposed the regeneration of the mass property the program feels that something is changed (even if nothing is changed...).

The next step is: how can I manage the file.prt of the hoses within whindchill?

Because if I duplicate an assembly the file.prt remains the same, but it changes only if I change the trajectory in the first assembly. So I have to make a new file2.prt.

The risk is to generate a chaos of external references...

No More has encountered the same problem?

There isn't a way to prevent the regeneration of the hoses?

What is the right way to manage them?

Any part that has a configuration that depends on where it is used is a tough PDM problem to resolve.

There are two ways I handle this.

On items that are simple I set the item to be flexible and then customize the assembled item using that flexibility. A typical example is a hinge - the opening angle is set to be flexible so that for each placement the hinge can be adapted. Windchill sees only one model and each assembly (or even multiple uses within the same assembly) can have a unique angle.

The limit to my patience is currently a motor with related capacitor which required the use of parameters to drive the location and orientation of a csys to locate and orient the capacitor remotely positioned from the motor. 6 degrees of freedom for the one component -> six parameters + six relations.

This becomes a problem when the amount of variation gets to be burdensome, so I would not use it to route a multi-branch electrical cable.

For more complex situations I create items that are of the form base-name_installed-assy. If there is more than one in a single assembly they would get a numeric suffix Therefore the item that has a unique configuration based on it's assembled location is named, in part, for that location. The file with just base-name is the undeformed/nominal geometry.

The Common name for all the variations can be the same and repeat regions can gather them to make a BOM with correct quantities.

As for regeneration - make sure the mass properties are calculated in the footer. I think if the mass properties relation happens first it is marked invalid when the external references are updated and is then recalculated. It's marking it invalid and then replacing the value that marks the part as modified.** When it's at the end it is simply calculated. Since nothing is marked as changed, the part isn't marked as modified.

**I have no access to source code - this is a description of what the software seems to do, not necessarily what the underlying process is.

Hello friends Do you know any software for linking 3d piping  to isometric drawing (or) generate isometric drawings  for piping's excluding "m4iso isometric for ptc".

Export to PCF is available out of the box.  Almost all isometric packages support *.PCF

thanks, jim

Announcements