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How to fix"Component Model Missing" err?

S

sparkfun

New member
Greetings,

Thanks to all you that helped my with my last question, this really is a such a great resourse only becuase of everybodys help!

My new problem, I have an assembly with most of the parts in one file but one is in my parts library. Everytime I open the assembly ProE cant find that one part, I get the error, I go to "quick fix" in the resolve feat box, find it and I am done. Well Im sick of doing that, can anyone let me know how I re-tell ProE to where to find it everytime?

Thanks,
sparkfun
 
Move the file that is missing to the same file that all the other parts are in. Pro-e defaults to a certain folder. If a part to an assembly isnt in that folder or the folder you designate when opening the assembly, you will get that error. Just save a copy of the missing part and put it in the same file as the assembly.
 
CPiotrowski said:
Move the file that is missing to the same file that all the other parts are in. Pro-e defaults to a certain folder. If a part to an assembly isnt in that folder or the folder you designate when opening the assembly, you will get that error. Just save a copy of the missing part and put it in the same file as the assembly.
Click to expand...
NO NO NO. Don't do that. The worst thing you can do in Pro/E is have multiple copies of the same part scattered around your hard drive. Sooner or later you will change one but not the others and you will start creating lots of headaches! You say it is a library part. If you installed the basic library correctly Pro/E should find those parts automatically. You can use the configuration file option pro_library_dir to point directly to the Pro/LIBRARY load directory.

If you don't have Pro/LIBRARYACCESS you can just add the config.pro option search_path to add the common files directory. You can have multiple search_path entries.
 
Dr & telecomguy,
Both ideas are good, Ive got one main folder that branches in to seven sub-folders and some of those have sub-folders as well. So I tried to write a config.pro file, do you think thats the best way? As well the file didnt work the way I hoped, here it is (written in wordpad and save in my loadpoint\text) -

# Search.pro for Pro-Engineer
# Casey Haskell
# Created 21 Feb 2006

"C:\Global\Casey's Work\Project Files
"C:\Global\Casey's Work\Project Files\10 pin LCD connector
"C:\Global\Casey's Work\Project Files\Bull tracker
"C:\Global\Casey's Work\Project Files\Graphics
"C:\Global\Casey's Work\Project Files\GSM
"C:\Global\Casey's Work\Project Files\IN2 Files
"C:\Global\Casey's Work\Project Files\IN2 Files\V4 and after
"C:\Global\Casey's Work\Project Files\Parts and Templates

The assembly file is in the second one from the bottom and the parts giving me the errors are in the last file. Also in my config.pro options I set search_file to the top file there and search_path_file to the above written file. Still no luck, any pointers? Thanks,

spark
 
< "C:\Global\Casey's Work\Project Files >


Spaces in the path along with the apostrophe look like trouble. I assume the single quotation mark at the front is an attempt to overcome this but I would expect a closing quotation mark. I've never tried this so I don't know that it is correct, but you might add a closing quotation mark. All my paths use an underscore instead of a space.


<tg>
 
Do not use spaces in Pro/E path names if at all possible. I would also avoid any punctuation like the apostrophe ('). You can work around spaces by enclosing in double quotes for some things but not for everything. Use underscore (_) to visually break up words where you want a space.

Remember, Pro/E supports multiple platforms (Unix, Linux, Windoze), most of which don't allow file name spaces and have different rules about restricted characters. Do a search on file name spaces, you will find lots of posts and workarounds for them.
 
Hi Casey


It used to be that you could not have spaces in the path. PTC would recommend using underscores instead of spaces. I don't know if that is still an issue. You may want to try taking the spaces out.


Sip
 
dr_gallup said:
NO NO NO. Don't do that. The worst thing you can do in Pro/E is have multiple copies of the same part scattered around your hard drive. Sooner or later you will change one but not the others and you will start creating lots of headaches! You say it is a library part. If you installed the basic library correctly Pro/E should find those parts automatically. You can use the configuration file option pro_library_dir to point directly to the Pro/LIBRARY load directory.
Click to expand...


I entirely agree with the Dr. if those parts are in a common file they are parametric meaning it have either a famliy table/vendor/part#/ect. and copying isn't a good idea for the reasons above. just add it to your search path and problem solve. Unless you save a copy with a deferent name in the same folder as the assembly then replace the part. BUT I'll still go with the Dr.'s option.
 
I tried enclosing each file name in quotes, didnt fly. So I re-named all my files with underscores instead of spaces. Still no love, when I open the assembly the parts still arent found. And after doing all that my working file directory is going to the default Pro-E one...grr :) Any other hints?
spark
 
add a search_path c:\the folder where your library parts are located in your config.pro file?


eg :


search_path c:\lib_parts\bolts


search_path c:\lib_parts\nuts


greets


nick
 
I was just giving an easy way to stop it simply by puting the missing part in the same folder. Alot of people dont necessarily know how to work with their config options. But, you are right, that is the best way to do it.


For the record, I donot support having multiple identical files in different locations. Kinda the reason why I use Intralink.


Good advice from these few users tho.
Edited by: CPiotrowski
 
I have many multiple copies of the same models. I do this because I don't want my existing models changing without control of it. I have a central place where I keep the current models. If I want my legacy data updated using these current models, I copy them to the location where they are used with a particular assembly. This gives me better control of what is happening with my existing data. This works very well for me.


I don't use Intralink, so I don't know how that would impact this management technic.
 
Morning folks,

I dont know what magical button I pushed but all of it is working perfectly, thanks for the help!

Spark
 
One clean way to make the parts library work on a Windows machine is to put the objlib folder in a path with no spaces and define all of the subdirectories with search.pro that ideally is also located in a path with no spaces. For example:

pro_library_dir C:\ProEngineer\objlib
search_path_file C:\ProEngineer\search.pro

search.pro file:
. . .
C:\ProEngineer\objlib\eng_part_lib\sl_cp_sq_screw
. . .

I believe the above can be accomplished if the library folders are in locations that contain spaces, but double quotation marks need to be included around all of the path names including those in search.pro. For example:

pro_library_dir "C:\Pro Engineer\objlib"

search_path_file "C:\Pro Engineer\search.pro"



search.pro file:

. . .
"C:\Pro Engineer\objlib\eng_part_lib\sl_cp_sq_screw"

. . .
 
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