Assembly Problem

[RandyGentry]

Ok if create a new assembly and then add a sub assembly(create it in the original assembly) then try to save it to a new folder it will save it. But if I close out of ProE and come back and open the original assembly it says it cant find the embedded assembly and I have to click on it and go and manuely find it. It does this with parts to. Any ideas on why. It really makes a mess of things to have all the parts in the same folder. Also using 5.000
This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[HatimAbdul]

The software is set up such that the assembly and all its components (parts and/or subs) must (by default)reside in the same folder as the top assy. In order for the program to locate components in other folders, you must define a configuration option (in the config.pro file) denoting the path to that folder. Repeat as needed for other folders. The config.pro can be edited and saved from the menu pick Tools > Options. The option name is "search_path". It might take a little bit of learning on your part if your company is new to Pro/E.

[RandyGentry]

ya coming from solidworks its a little different. Thanks!

[RandyGentry]

is it possible to turn of versioning of files

[HatimAbdul]

I'm afarid not. But you can easily clean up your working directory (within Pro/E) using the purge command. Click Window > Open System Window. the DOS prompt will come up. Type "purge" and hit Enter. This will delete old versions of all pro/e files in that directory (keeping the most recent ones.) I'm assuming you're not using a PDM program such as Windchill.

[RandyGentry]

no I'm not. Its just the student addition. I'm learning it so I can hopefully have a better chance of getting a job a certain company that I want. Also planning on releasing a product in the next few years and I learning to use it for that. With that said no I don't have windchill or anything like that. Thanks for the help though the purge command is works fine. I just hate having tons of old files.

[AnkurAggarwal]

Regarding ur assebmly problem, if u backup the assembly instaed of creating a copy in a new folder, then ur problem will be solved. As all the parts/subassy are copied into new folder when u backup the assembly. Ankur

[RandyGentry]

Wow thank, I was just coming back on here to post the the way stated above was only working for my some times(until I restarted ProE) then I would have to delete the old option and re add it and then it would work correctly until I restarted again. I tried your way and it worked like I wanted. Now I just need to make sure it works when I restart the computer. Man ProE is so odd how it does some things. It sure does beat solid works in performance and usefulness though. Just kind a quirky and hard to figure out at first. That's the main reason I learned solid works first though.

[RandyGentry]

Wait all back did was save all the files in the main directory. Is there a way to have then save in a sub folder. Just curios should I just save them all in one file and stop bothering with it. I used the folder and subfolder thing in solidworks to make it easy to fine files. But in solidworks I didnt have 10 of the same file all looking th same. Is there a better way to do what I want or should I just save it in to one file. Thanks!

[AnkurAggarwal]

When u backup a file (assembly, part or drawing), it creates a copy of all the files associated with it. For example, if u back up an assembly, it creates a copy of all the parts and subassemblies in the main assembly. and backup is used to create copy of files in a folder other than working directory, as u want it in subfolder.

[RandyGentry]

yes and I tried it but it but it copy's ALL files into one. So it kinda defeats the purpose. As well I still have to search for the file when I start ProE. Am I doing something wrong is is this correct.

[ptc-1972305]

First you take the back up (Don't use save option) of top level assembly in new folder let's say XYZ. Now restart your proe (If you want) and then open top level assembly from folder XYZ. Hope it will solve your problem. Regards, Vimlesh

[ReinhardN]

Randy, you really should follow Hatims advice (search_path) The load sequence of ProE is - memory - working dir - search paths in given order once the component is found, the search ends. You will find further information in the help files. Dont use the backup solution as it will set the revision number to 1 and will leave you with multiple files of the same component. This will bite you later on. - versioning: ProE will not overwrite files when saving. You will appreciate this behaviour as you can always go back to a previous version when something has gone terribly wrong. Typing purge in the system window will delete all old versions in your working dir. If you want more comfort, you can use the SpekanPurge utility which can recursively purge a folder tree. Reinhard

[RandyGentry]

I tried the backup thing and it worked but it just took all my files that were in sub folders and in the main directory and put them all in the same(new) directory. Does not solve my problem of separating my files for organization purposes. I also tried the search_path one a few times. This is exactly what I wanted to do and it works(SOMETIMES). Im not sure if there is some bug in 5.0000 or what but it will work for a little while then it will not work and I have to go in to options select the option and delete it then exit options and reenter options and then find the search option and reset the directory that it searches for and then it will work for a while longer. Any thoughts as to what is going on. I also have some circular references files in the directory. Are these good, bad, ok or what.

[ReinhardN]

Hello Randy, you need a separate search_path statement for each folder. Blanks or special characters in paths (e.g. My Documents) lead to trouble as the search path may not be recognized. Remember the search order. If you want to load a file via search_path which you already have in in memory or working dir or in more than one search path, ProE will grab the first one it finds. So it is important to have each component in one place only. Circular references may lead to crashes, so you have to fix them. Reinhard

[RandyGentry]

well so far all I have is one sub folder which is C:\Documents and Settings\Gentry\Desktop\ProE Snowbike\Rail is this not right? as for the circular references how do you go about fixing them. Is there any info on PTC university because I have access to that. Sorry for all the newb questions but I want to start using proE the right way so that later on I don't have to completely rebuild my project from scratch a few times. I went through that will solidworks and dont want to do it again if possible. Once agian thanks for the help!

[HatimAbdul]

Like Reinhard said, you're not supposed to use folders with spaces in their names. Also folder paths are case-sensitive. Create as many search paths as needed for all your folders where you want to keep your parts. PTC offers web-based classes, as well as instructor-led. But they may be expensive for you if you have to pay yourself. The search path issue is also so specific it won't be covered in a particular class. I suggest the Help Center (within Pro/E) as a rich source of information and education.

[RandyGentry]

Ok so since Im not suppose to have spaces how do I stop that. This was what the default windows gave a folder that was on the desktop.

[RandyGentry]

ok I figured it out. I moved the main folder from the desktop to the C drive where program files, system, etc and it worked perfectly. It kinda suck as I like to have my current projects on the desktop but cant be to picky I guess. While I have you I have been searching and cant find an option to set what you have displayed on start up. Like datum plains, axis, coords. Is there one to change them or do you just have to turn them off before you start. Yes I realize I am being picky but I just want to get an idea of what I can do. Thanks alot for helping with the sub folder issue.

[ReinhardN]

@Hatim, I dont think folder names are case sensitive as it is a windows function, though sort order in ProEs open window is affected. @Randy you know that c:\documents and settings\gentry is user specific which means if you log in under another user name you have no access. If you are working solo, its ok. If not better place your data somewhere else. For search path reasons better use something like c:\CAD_Data\Gentry\..... Reinhard

[HatimAbdul]

Hallo Reinhard, You might be correct. I used to think it was not case sensitive till my boss once had a problem connecting to the formats folder automatically till he found out about the config option to the folder path was not edfined with the same case as the actuall path. Again, you may be correct. I'll have to experiment with it.

[Kevin]

You can use directory locations with spaces but you need to enclose them in quotation marks ("..."). So you could use the folder on your desktop in a path name.

[RodneyDecker-di]

"Randy Gentry" wrote:

Ok so since Im not suppose to have spaces how do I stop that. This was what the default windows gave a folder that was on the desktop.

[RandyGentry]

about the crc file. I looked into them and fix a lot of them but some i don't know have. For example I referance a surface on a part in the sub assem to a part in the main assem as a pivot. Then I get a crc that the reference has to wait until the part within the assem is figured out before it can determine how the pivot should function. But this is kinda what I want right. I want it to figure out the dimensions of the part in the sub assem first them figure out the pivot. Any ideas!

[DavidButz]

Randy, You do NOT want to have the kind of dependencies you just described; they will cause you grief down the line; it also means that you don't have the kind of maximum independence you would like for various parts and assemblies relative to each other. There are great techniques to do what you want including Skeleton Models and other tools covered under the topic of Large Assembly Management. To get started, however, try to create Datum & Surface references at the top level, then refer to them at lower part and assembly levels for assembly, etc. This is a general and vague answer, but it's an important issue. David

[RandyGentry]

Hey thanks. I actually figured that one of my own. I started constraining all my parts before I even made them with datum features. Also I have been trying not to get into advance assem features because it is a extra addon that cost quite a bit.

[DavidButz]

Hi Randy, Good for you figuring the datum technique out on your own! Yes, it's irritating that you have to pay so many $'s for the Advanced Assembly extension. However, some of the techniques are still possible. For example, the software won't recognize and handle Skeleton Parts in an automatic way without the extension, but you can still use them; in "the old days", before automatic handling of Skeletons, it was already a technique. (You just create your own part with Datums, Surfaces, Curves, etc., add it as the first part in your assembly, then "hang" the parts and sub-assemblies on the skeleton like a hatrack. You can incorporate motion relationships into your skeleton, too (swing a Plane around an Axis, and your assembled parts will move with it). David

[RandyGentry]

ya it works really well and reliably now. I just how to go back through the whole assem and redo ALL of the parts. Its taking forever but so worth when I can just type in a few different parameters and change all the parts without having to think. Then I just grab some and start moving them to see how they interact. I have access to to PTC university so I will probably go through the advanced assem module as well as the others as I get time. I'm pretty sure once I get all the parts I have done redone making new parts wont take that much time.