In the 2d drawing are flat states. See the figure. Whit the "save as" commando I can only rename the normal parts. There is no dialog box or something where I can rename the Flat states. In the new drawing (2d) is the folded part renamed, the flat state not. Creo can't find the flat state and the 2d file will not open.
It goes like this:
1300670-0168.prt new name is sample-0168.prt
1300670-0168_FLAT1 does not exist in the new working directory. It probably still exist in the old working directory because I can open the original drawing.
Flat states are typically saved within the model as family table items. They appear as flat states but they're really just instances in a family table that belong to the model (part, not the drawing). When you do a Save As on a family table, the instances are not renamed when you're working outside of a workspace.
If you're working within Pro/E's data management tools, Windchill, your workspace is intelligent enough to realize that your model has a family table associated with it. You can use tools within the workspace to rename the parent model (also called the "generic") and the family table instances at the same time.
When you're working directly off your hard drive you have to perform this renaming manually. It's hard to describe this process in an email without making it all sound confusing. Do you have a part and drawing you could share with us? I can use your part and drawing to make you some slides to demonstratre the steps to perform a Save As without losing work and without having to delete any views from your drawings.
Managing ProE's files without data managment tools is horrible. You can't automatically create drawing with same name as part, open drawing with name of active part and you can't create save a copy of assembly with flate states.
We tried everything, but at last (PTC support in our country said this too) there is just option to do this manually. I create one mapkey in WF5, but it didn't work fine (somtimes, when was there files with too long names it has problems, so I didn't work on them later, because I hoped it works in Creo 2 (now I have Creo2 and I'm really disapointed, just new cover, but same bugs and problems like WF, so I counting down days until I will start working with new cad software)
Like BrianMartin mentioned, Flat States are family table instances. Managing them without PDM is a tuff work.
Unfortunately when you Save As a generic part there is no function to provide Instances renaming unless you are on PDM. So new copy of generic will have same old name of flats (instances).
But when you Save As from assembly and have generic parts in assembly, it is different : new copies of these parts will have Family Table completely stripped of it (no instances, no flats etc).
You did not explain exactly which models does your drawing contain (only flat instances of parts ? both formed and flat parts ? so guessing).
Suppose you have drawing FORMED.DRW with views of both Formed state (generic) and also Flat State (Instance) of the part. FORMED.PRT (with FLAT instance) is a part of your assembly.
Case 1. You Save As your assembly to new name / new location. And rename FORMED.PRT to FORMED_NEW. PRT . Drawing FORMED.DRW copies to FORMED_NEW.DRW, and you get FORMED_NEW view alive (since FORMED_NEW drawing model is alive), while FLAT view is "dead" (since associated with it FLAT instance got stripped upon assembly save-a-copy).
Well the only way here - re create new FLAT state in FORMED_NEW. PRT and add its view on FORMED_NEW.DRW.
Case 2. Now all the same, but you Save As from the FORMED part itself to FORMED_NEW.PRT. Drawing FORMED.DRW copies to FORMED_NEW.DRW, and you get both views alive : FORMED_NEW and FLAT (old name of instance remains). You have drawing with all views alive. FLAT can be later renamed through Family Table to another name, and with drawing in session views will update.
But if you save individually several parts with flats, they will not get to a new copied assembly without your extra efforts. After you Save As assembly and all components to new names, (say FORMED.PRT -> FORMED1.PRT) you will need to Replace them one by one with those you copied for the flats. Means you will have to open your new copied assembly, select FORMED1.PRT and Replace "by Unrelated Model" with FORMED_NEW.PRT, mapping all references. This is not an easy task.
To my knowledge, these are the two options if you do not Save As from PDM system ...
Thanks for the reply. We are now thinking about placing a flat state in a drawing, export a dxf and delete the flat state. I have made a mapkey for it. It is not the right way and it feels a bit like giving up, but for now, it is the best/fastest way.
I used to draw whit Inventor. Making a dxf and a flat state was very easy. Right click on the flat state and “save as”. No fuss whit creating a “new” part, or import a flat state in a drawing only to export the file…… oh what a wonderful time was that….
Next month we have someone from our software supplier in the office for simulate. I will ask him for this also.
We copy/rename drawings with sheetmetal flat states on a regular basis, the method we use is:
Open drawing - perform file>backup (not save copy) on drawing itself into a new directory - this will automatically backup all models assigned to the drawing into that new directory.
Rename all files in the new location (you will need to go into the sheetmetal family tables to rename the flat instances). Make sure the drawing is in session when renaming the files.
I know this is a pretty quick explanation, let me know if you have questions.
I'm hearing a recurring theme here. Indeed, as I stated above, it is a time honored method with Pro|E to load everything into memory and rename in a logical manner. With the updated save-as dialog in Creo, some of the old methods are not as easy to comprehend but they work.
However, having said that, Vladimir, you do see how the Save-As dialog lacks one element that needs to be addressed by development!
Stefan; it is sad to see the use of an imported DXF as a "solution". I would almost rather have the flat state as a second Creo file (maybe even associated to the original somehow).
Antonius, , note taken.
Small comment here : any solution with recursive renaming will be a complicated solution for the user. If and when we go this way, while Renaming assembly structure user will have to manually visit dozens of Generics (that are Renamed), expand their Family Tables (that can be huge) and Rename all corresponding instances. Then Drawing that uses such Instance might survive [also only if it has other "straight forward" Renamed drawing models (generics).]
PDM is tuned to address such database tasks easier way.
Good point. Indeed, the case of flat and formed sheetmetal is a fairly common case but only a small subset of the bigger family table picture. I would hope that people using large family tables for their product offering are more on the OEM level where next level assemblies are limited. Personally, I have survived decades without the need for family tables.
We already have an enhancement request in for another sheetmetal problem when it comes to how the master model is presented. The logic of the software and the real world usage is not exactly in line. When you assemble sheetmetal parts, obviously you want them in the final form, preferably, the master model. But for drawings, you often want both, flat and formed. If the model allows for a bend back feature, no issue, but if you need the "full" flat pattern feature for the drawing, your master model will be flat. This just goes against the grain and we have to resort to family tables. Generally, we simply need a re-form flatpattern feature much like the bend back so it can remain as the last feature in a sheetmetal part. This would allow for display states in drawing views to manage flat patterns rather than family tables.
But it does beg the question, why can't the Save-As dialog query and manage family tables? As much as these are part of core functionality, managing them should also be.