File location & Mass Properties

[ptc-4339982]

I have created an assembly in Creo 1 with various parts from folders on my G: Whenever I start Creo and try to open the main assembly certain parts will always require me to retrieve them, I then have to naivgate to each folder in the working driectory to find the missing parts. The parts which are in the same folder as the assembly are found however the parts not in that folder cannot. The working directory is set to G: and none of the parts have been moved since the assembly was saved.

Why should it do this?

My second question is about mass properties. Whenever is ask for them to be reported I get an answer in tonnes and also properties such as density are reported as tonnes/mm. This occurs no matter what units I set the material to.

Is there a way to change this to more useful units?

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[JonathanHodgson]

Steve,

I'm working with WF4 so some of the terminology or locations may have changed. Hopefully the principles will still be the same.

1. Pro/E assemblies only save the component names, not their location. When you open an assembly it will look in the directory the assembly was opened from; then the working directory (I think that's the right way round) and then it will look through the locations in a search path file (ours is called search.pro) which you can set a pointer to in config.pro (search_path_file z:\search.pro).

If you have standard part directories, or you pull parts from multiple different projects (as we do) then these locations should be listed in search.pro. Be aware, however, that having a very long search path can slow down certain operations such as new file and rename; and the order you list locations is the order Pro/E will look through them, so put little-used ones at the end. Also, Pro/E requires any filename to be unique within the search path - you can't have two models with the same name. If you do somehow achieve this, Pro/E will just open the first one it finds and try to put that in your assembly.

As a side benefit, if you use File->Open you can simply type a filename (e.g. widget.prt, tool.drw) and Pro/E will look through the search path and open the file without you needing to navigate to its location.

2. You can change the units set for the entire model, via Edit->Setup in Wildfire and earlier. However, think carefully about which units you want to use, and why. For a long time we used mm, kg, sec; but when we started using Mechanica this meant that force would be defined in kg.mm/s^2, which I think is mN. Instead, we switched to mm, N, s, which gives mass in tonnes (as you have) but means that forces are in N and stresses are directly in MPa.

To 'fix' the reported weight on a drawing, we use the relation WEIGHT = PRO_MP_MASS*1000 in our start part and then display &WEIGHT in the drawing border.

[linda]

hi

i tried to add searching path before, and found that for search path g:, pro-e just search files in g:\ not in g:\xx.

for the unit, choose setup-unit management, copy the one you are using and edit to set the unit as you wish for mass ...

th default setting fot mmns for mass is tonne.

hope it helps

linda

[KshetrabasiMaha]

Hi Steve

there is a similar discussion on Assembly with parts in different folders

http://communities.ptc.com/message/162514#162514

this will help you to create your own search path file

few points I want to inform you

1. try to use search path file in current season config before start working

else if you use it in default config.pro it will always search parts in those folders

it basically depends on your requirements

2.if you have never made a search path file ; then you need to make a file in note pad file and rename the extension from .txt to .pro

regards

k.mahanta

[BrianMartin]

Hi LInda...

The search path file is not recursive... you literally need to specify each individual folder you want searched. You'd have to specify one line for G:\xx and then another for G:\xx\yy etc.

This allows you to search folders in any order you specify. As others have pointed out, Creo will search the paths in order and open the first occurrence it finds of the models you need. Many users get in deep trouble when they have multiple versions of the same part located in different directories.

Me and my colleages call this method of working the "Wild West" style. Although we utilize Windchill for the vast majority of our users, we have some stragglers who absolutely refuse to use it. They work "wild west" style with subfolders on their c: drive acting as their data management system. In doing this they lose the power of Windchill. They also lose the safety of Windchill.

Working with folders on a network or local drive is tough. If you need to maintain revision control it gets exponentially harder. Attempting to keep multiple revisions of a part necessarily means you're trying to save the same model in multiple places. As soon as you do this, search path management becomes critical. If your paths aren't maintained well, Creo might come across rev "A" of a model in the seach paths before rev "B" or "C" thereby causing a ripple effect of problems.

If you have difficulty getting the search paths to work or creating a search.pro file, just let us know. I'm sure any of the people on this thread could help.

Thanks!

-Brian

[KshetrabasiMaha]

Hi steve

Some of the options are at different location than WF-5

For Config.pro

It is in

file > options

Model properties is in

file > prepare> model properties

Regards

K.Mahanta

Message was edited by: kshetrabasi mahanta (images added)