Need help with drawings in Creo 2

[ptc-3116419]

Okay I'm in Pro E Creo 2.0 and working on a drawing. I normally work on NX and these two do not work the same. The original assembly I set the drawing to was named incorrectly so I did a save as on the assembly. I am trying to replace the old assembly in the drawing with the new one that has the correct name and it's a big fail. I am able to "set" the new model in the drawing but cannot get the views to update to the new model. Now this drawing pulls in both models if I close and re-open it. I am unable to delete the old model from the drawing without getting the error "Cannot delete model with views using it" How do I get rid of the old model and update the views to display the new one?

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.

[JamesBurcham]

If the model are not part of the same family table or interchange they will not directly replace. If you are replacing a model in a drawing with a completely unrelated model you are almost better off just starting a new drawing. To remove a model from a drawing you need to remove everything related to it. That means all views that contain that model, and any notes or tables linked to that model.

[ptc-3116419]

I've been on several different CAD systems over the last 20 years and ProE has impressed me the least. User unfriendly and remedial. What takes 4-5 pokes in NX or Catia takes at least twice that in ProE or the task can't even be done at all. As simple a thing as replace a model in a view cannot be done. Shame on PTC.

[ReinhardN]

Why dont you

- rename the assembly to the old name

- open the drawing

- rename the assembly to the new name

- save drawing and assembly

For renaming you must have all dependent objects in session. ProE will correct all dependencies for you.

And dont forget to save.

[rohit_rajan]

there are many things extremely good in Creo(ProE)....if you keep comparing with NX you will be dissapointed...so try to do it the Creo way....and you will have less issues.

[dgschaefer]

Assuming that you are not using Windchill or another PDM, an easier approach would have been to open the drawing and any assemblies that contain that assy and use the rename command in Creo. Then all objects that refer to [old].asm will now refer to [new].asm.

If you've already replaced the old assy with the new everywhere but the drawing, you can trick Creo into using the new assy using the method Reinhard suggested. To clarify, you open the newly named assy, use the Creo rename in session function to rename it back to the old name, open the drawing, go back to the assy and use the Creo rename in session function to rename it back to the new name, save all.

You shouldn't loose anything with either method.

[ReinhardN]

As you can do much damage with renaming I usually work with copies in a separate folder after I have erased all objects from memory. If everything was successful I copy them back to my working dir.

Reinhard

[dschenken]

If it worked just like NX it would be NX.

The reason for Creo not to replace models in views with unrelated models is that the view structure begins with the model - orientation, scaling, sections - and without those things the view no longer exists. There are special cases where a model can have variations, such as family tables, that have suitably identical structures and can be easily replaced.

You could have created a temporary family table in the original item, replaced the model in the drawing from the family table, then deleted the table and, in saving the drawing, saved the new model with the new name. I have to assume that you wanted to keep the wrong name model and the right name model, otherwise you would have just renamed the model.

Still waiting for the software endpoints analysis so that users can see what they know and don't know and can search them for results they want so they can backtrack on how to get them. Someone should have written them down before developing the software; they don't just pick a bunch of steps and then say to themselves, 'what should happen now?'

[TomD.inPDX]

So here's a question... how do templates deal with predefined views when the model changes on creating a new drawing?

[dschenken]

Here's a better one. I searched for NX views to see just how easy things are over there and found

"As Cowski mentioned projected views are not associative with their base views once that they have been added to the sheet. Section views are dependant upon how the section cut is defined as to some extent are the detail views upon boundary definitions. I think that the sheer complexity involved in re-orienting views as you appear to suggest invites a number of problems that may challenge the drafter's ability to confidently control the results, which is why I don't find myself warming to the idea."

The rest is at http://www.eng-tips.com/viewthread.cfm?qid=271309

[ptc-3116419]

Cowski's answer is correct and has been a complaint by NX users before. You should be able to easily flip a view from say a plan to a bottom view (Which actually is easy in the edit view>orientation mode) and have the projected views flip likewise.

[dschenken]

The templates depend on coordinating pre-defined views of particular names with matching names in models in order to place and orient the views. I'm not sure what happens if there is no match.

After the drawing is created there is no guarantee that on any particular drawing the views in one model would match those in another, even if the names matched. When it happens, it's a special case. It's similar to why it's not possible to simply go to the model tree and simply edit a part name as a simple way to simply substitute a new part. Seems like it would simply work for simple things like washers and bolts and nuts, but it simply isn't simple at all.

I think if one was careful one could use templates, but I never ran into users who were so fastidious that they would make sure the Front view was always something sensible, so I typically ended up deleting template driven views.

[TomD.inPDX]

You would think a replace similar to assembly component replacements could be implemented fairly easily in drawings.

Maybe PTC just forgot that the current functionality is somewhat archaic

[dschenken]

It's a slippery ugly slope.Should all the components get balloons that match the function the parts provide, all the dimensions be layed out the same as they were? If a view has sections with it that the replacement doesn't have, should the replace function create those sections?

I just see that when this would work well enough to make it OK is so rare as to by useless.

The only reason this could possibly work here is the original approach to the simple problem of changing a file name was not to simply change the file name, but to do something else.

This is a great example of the XY Problem I posted about recently. Have problem X, try solution Y, solution Y fails, ask for help with Y. Fortunately, the original problem statement included a mention of X.

[TomD.inPDX]

Oh yes... I can see the slope is pretty steep!

However, my use case is quite common and even if all the dimensions unassociated or disappeared, I would be happy if only the drawing "setup" remained for the most part, even if aliased for the moment. Drawings handle aliassing pretty well*.

My use case is when you have a part file fully detailed and some yahoo decided they want to add an OEM hardware widget. Now you have the same drawing but it is an assembly. Of course, I am going to have the same parameters to fill the tables, and I even have the same base part from which the dimensions can be shown (that might be asking a bit much)... Even the view orientations can be "frozen" to the default CSYS or use the datum references if the name doesn't exist. If you reoriented the assembly in relation to the part, well, duh, it will reorient the view... but if you did your due diligence to make sure the names coinsided (only the general views need to match), then this should be a pretty simple process of eliminations. It can require the user to redefine any view related issues after the fact.

I have been caught in this dilema more than once. There really should be a consideration for this. I have gone so far as to make single part assemblies just to get ahead of the game. A sheetmetal part where someone desides they want to add a single Pem fastener, for instance. Do you realize just how much work that one "little" change can mean?

The rename trick is not going to work in this use case since the extention changes from .prt to .asm.

* ...at the moment in instances such as changing the orientation of the master view, allowing you to fix the dependent views and eventually everything falls back into line.

[dschenken]

I've also wanted a flatter modeling system for a long time, where parts and assemblies weren't different, for just the same reason. Plus, it would make adding material to assemblies easier. Real solid welds, for example.

For example: ready-to-use casting and someone comes along later and wants to add an insert or a sticker.

On drawings I'd just add a new dash number and views showing the assembly of the items; I don't see a need to remove or replace existing views of the base component. It's the higher assemblies where this becomes a problem. Not only does it require replacing and rerouting, but all the next higher assembly drawings need a close inspection for leaders that no longer point where they should and repeat regions that need to be repaired.

I'd toyed with the idea that there would always be an assembly for each part, but that screws up the PDM side and makes a lot of other activities harder. For certain someone is bound to rename the part and not the stand-by assembly, leading to a lengthy search for which name is correct.

[TomD.inPDX]

True; in many instances I detail the part and add the inseparable press-in feature in a separate view with a different model in the drawing. I don't use a PDM and therefore don't have to account for build levels, and the part and assembly can have the same name.

However, convention for sheetmetal as an inseparable assembly is to show the hardware in all views. Even the opposite has happened where the only Pem hardware was threaded fasteners and the manufacturer offers a great discount for using pierce and extrude - tap options. Suddenly it goes back to being a single part! Fortunately this is easier to solve as I just leave the assembly in the drawing. I generate engineering requirement drawings, so I don't concern myself with the shop practices. I don't generally offer flat patterns either. I might use them as reference for specific detailing requirements.

All in all, I like the way Cadkey dealt with views... "it's just a viewport into space". You put 3D stuff in front of the port, and you see it.

Obviously there are challenges to changing models in drawings. But it is clear to me there is a need for it. As "Z" argument... I can see composite capabilities in part files to deal with this but even that is a long shot.

[James62]

Hmm, not tested but the only solution I can think of would propably be to add (import) the sticker or nut or whatever as another component to part level, and then for BOM just use dummy empty part that contains all the necesarry parameters of the added component.

Not sure how would the hatching on such multi-component part drawing xsec look like, but I guess it's worth the shot.

If you wanted a small BOM on such drawing then, you would just add the assembly model with both the original part and a dummy empty part, to the drawing just to generate the table from.

Also, Repeat Region can be set such that it can deal with lots of the unusual irregular parts, assemblies, components. It "just" requires some serious setup.

To answer the original question, well, maybe... Have you tried to replace the actual part file, named say XY with another part file with the very same name XY in the working directory, and then open the drawing associated to this said part name XY? I've never tried that, just wondering what would it do in your case?

[TomD.inPDX]

Making hardware for sheetmetal part in part mode is not an option. I do provide STEP files to suppliers and I do want the supplier to be able to remove the hardware for their process. There really is no easy solution. The preemptive solution of creating an assembly for the drawing is likely the safest method.

Also, if the original part is sheetmetal, you cannot even merge a hardware component into it. It has to follow that "thickness" rule. In part mode, you typically also need to distinguish the "head" of a flush fastener... meaning it has an outline that would merge and vanish in part mode.

As a rule, even when a part is an inseparable assembly, make it an assembly. Having the sub-category of "inseparable assembly" would be very nice in Creo. It can be a distinction for PDM to consider it an assembly without a structure below it.

In every CAD system I have ever used, including NX, you would have to "fake" the system one was or another to manage product structures including PDM systems. Most PDM systems have a way to compensate.

Here is a great example. You have an OEM "part". Is consists of a body, lock washer, washer, and hexnut. It is all stocked under one part number but it is important that the drawing show these 4 items exploded, not to mention that assembled, the panel it is installed in can be of any thickness within a range. Oh, and we need a cross section too (while we're at it ). How do -you- structure your model to do this?

I have one part number for the OEM component... 12345

I need 4 sub-components and an assembly; 12345-1.prt 12345-2.prt 12345-3.prt 12345-4.prt 12345.asm

Today I can use flexible assembly feature in Creo to move the nut, washer, and lock washer to the right location and install the 12345.asm part. in the past, or in other systems, I would need to assemble the parts themselves and a blanked assembly to cover the PDM. And I can explode this part perfectly, and I can have appropriately cross-sectioned views. Life is good. However, if the part was an "inseparable assembly", the assembly would know not to have -any- structure below it... automating the PDM structure reporting and have a flag for repeat region BOMs. In my book, this would be the next best thing to creating "composite" part files.

[James62]

Ah, right. Only surface models can be imported or merged into sheetmetal parts, and surface models or quilts are just bad for drawings. So, that's no go if you want to keep the history tree intact.

Heh, I still think it's possible to turn part drawing into a fake assembly drawing. It just takes some twisted effort. For the STEP assembly file for a supplier you can make a separate assembly that can have the right structure. I realize that means duplications of the same geometry, but that's the way it goes.

For an unbent state, you can make a separate model as well, and that would be the only thing you would need to replace on the drawing. Sounds like alot of trouble.

For OEM parts I usually go with safest method, that is have it as an assembly, even when it comes from IGES file and shows as one part after all. For an assembly drawing then, I always make sure to split it up into separate parts so the cross section is correct.

Actually, when I get a part like that i usually use Rhinoceros for help cause it's alot faster to deal with dead data containing just a bunch of surfaces there. In Rhino it's easy to make and name separate closed polysurfaces from a pile of surfaces that kind of touch or even overlap each other, mainly cause Rhino doesn't work as solid modeler. From there i save it as a STEP file, and import it into Creo.

It's just a bad input that needs to be corrected first elsewhere so Creo can deal with it.

I like the idea of changing prt files to asm, and back, even if it means loss of some of the features, cause not all the part features are applicable to assembly (why is that anyway?). After all any of these is just a node in a structure tree.

[TomD.inPDX]

I got the sheetmetal flat pattern down pretty good as long as you don't need forms flattened.

Creo 2.0 Sheetmetal - Simplified Reps for flat pattern drawings

This maintains the flat pattern as a simplified rep while maintaining the master as the formed part.

It is not worth messing up a straight forward associative process just to keep from doing a little drafting. It is just annoying when you face re-doing a perfectly good drawing just to switch from a part to an assembly. One thing that is good is that the driving dimensions from the model are already set to what you need... IE: the annotation additions in dimensions are still in tact in the model. Drawing annotations can be -redirected- if you maintain the original view for the moment and reassign references. Move to view also helps where it support this. In 3 years, I may have done this a half dozen times.

[ptc-3116419]

I'm not asking it to work like NX, Catia, Solidworks or Autocad, I just want the system to use a more common sense approach. I'm not going to go thru all the differences because there are to many to list except to say that the other systems I have been on use a similar approach to modeling and drawing creation where as Pro E has it's own little world. A few years ago I worked with a company that was switching over from ProE to NX and after about 6 months of learning the operators most( about 45 out of 52) of the designers preferred NX and some had been on ProE for years.

When you turn the steering wheel of a car left the car goes left and likewise if you turn the wheel to the right the car goes right. If PTC designed the vehicle then when you turn the steering wheel to the left the car would go in reverse.

[dschenken]

What does NX et al do with what I suggested before?

"Should all the components get balloons that match the function the parts provide, all the dimensions be layed out the same as they were? If a view has sections with it that the replacement doesn't have, should the replace function create those sections?"

And what happens to all the next assemblies and their drawings that still use the wrongly name component?

I can't imagine NX fixes all that simply or easily.

[dhermosillo]

@Jeff, are you using Creo stand alone or in a linked session with Windchill?

If it is the former, then any of the aforementioned methods will work.

If you are using Windchill, select both the drawing and the model in your workspace and do a save as. This will copy the drawing and the model to a new drawing and model. The last step is to go into Windchill and rename the the files to what you want them to be. If you aren't going to use the original anymore, we usually just append it with _obsolete.

Keep in mind that Creo/Windchill currently has a limitation that will not let modified items be copied. I know it's stupid and I've filed a ticket with PTC, but they refuse to acknowledge that it's a bug. It is particularly annoying since that is how a lot of new iterations happen; you start to modify a model and then realize it should be another part entirely. PTC has no easy way to accomplish this right now.