I have a drawing which I copied and renamed. We are currently creating a development drawing and then later a production drawing in which we use a different drawing number. I want to replace the model in which the views are created from with an identical model assembly with a slightly different part number. I've tried the "Drawing Models" commands and I've added the model, so it shows up in my list of models. I've tried to use "Replace" but it doesn't seem to work. How would I go about doing this and preserving my views and dimensions, etc.? Thanks
You could take the original drawing and original assembly, and produce the new drawing + assembly with Rename. If you don't do something like that, you have an assembly that you say is identical, but to Creo it looks unrelated, and replace -type functionality will be unavailable or strip out any references, or if you try to cheat the system, you could end up with references that are to the wrong type of item entirely (for example, information on a shown axis, but when you look it up in the part, it's an edge made by a cross-section). That can cause all sorts of trouble, so don't try to cheat it. Instead, copy both the drawing and the assembly so you have newdrawing of newassembly, and then you're set.
This is really an area with no reliable answers. The tools to repair unlinked items just don't exist. And it is really a big problem if PDM is involved.
I have resorted to a side-step to get the correct names et al for assemblies and drawings to avoid repeating thousands of mouse-clicks to put items back to where they started when low-level parts are to be replaced in an assembly structure that is multiple levels deep.
In my case, both the original and the new name drawings must be maintained as the existing ones are in production and the new ones need to go through the release process. Common changes require double work, but that's how it goes.
The replace command in the drawing only works for family table driven models, as far as I know. It won't work on models that are copies of each other.
Another issue you'll have is that by default Creo stores some of the drawing info (created dims for one) in the model file rather than the drawing file. So, by swapping models you'll lose some of the dimension info.
You can trick Creo into using the new model by saving a copy of the drawing to an empty folder, saving a copy of the alternate model into that folder and then manually renaming to the original model name. When you open the drawing Creo will find the old model name and use it for the drawing, but it's pretty likely that a lot if things will either be missing or wrong.
The best path is to put off the creating of the production copy as long as possible so you have the most "mature' development model possible. Then you use the backup command to create a copy of the drawing and all models in a new folder. Then, starting from a fresh Creo session, open the new copy and rename the drawing and model(s) accordingly. You can then use the backup command to put it back in the main folder.
It's important that you fully understand how Creo retrieves files and what happens when you use the backup command as it's pretty easy to mess things up if you don't All that assumes you are not using a PDM system, if you are, much of that should be done within the system. I'm not familiar with PDMLink to give you directions on that.
Another path would be to not make a copy but instead just transition your development model into production, but I assume that your company policy prohibits that.
A colleague points out an obvious answer I missed.
If you open your model (part or assy) and if the drawing and the model have the exact same name and you have the config option "rename_drawings_with_object" set to "both" (it defaults to "none") and save it to a new name, then Creo creates a new copy of the assy with a new copy of the drawing both with the new name you supply.
You can add drawing in new sheet with insert--> import drawing/data, where you will get new model & drawing. Once you are complete then you can delete first sheet and associated model. I think it might help you..
yup ran into the same issue was forced to -recreate the drawing with a similar part.. pathetic,.. in SWX you can easily do this.. the dim's need some cleaning up but you don't have to start from scratch
As usual it feels like insanity when you're working in Creo and try to do something that is basic functionality in SWX and creo offers no solutions. I'm adding it to my list of things swx can do that creo can't.
If you are allowed to do it, create a family table so you can use replace. If things are similar when you use replace any features that have dimensions should keep their references. If features are removed the dimension should turn purple. If you leave the dimensions on the drawing and replace the model with an instance where the features are present the dimensions should regain the references. There shouldn't be a need to start completely over but it may depend on company practices.
So do I have to plan ahead if I want to replace one similar model with another.. Is it straightforward or more of the unintuitive/ convolute setup?
Depends on what you are trying to accomplish and how you view it. If you are wanting something that stands by itself you may just need to copy the model and drawing the similar part is based off and modify from there. If you want a connection between the base and similar parts then a family table is needed. You copy the drawing of the base part and use replace in the new drawing to specify the new instance. Shown or created dimensions that are the same between the two instances should remain on the new drawing and you should only need to create or show new ones. Either way things aren't being created from scratch but you may need to provided more info about what you were actually doing and why you needed to start from scratch. Just based on the description(s) I'm not seeing anything that would cause you to have to do that.
I have used this from time-to-time. Create a temporary instance, do the replace and then delete the table and save the using assembly. If possible, keeping the instance is a great think, but then it runs the risk of mismatching release versions.
What is -very- important is to delete the table before saving the using assembly, otherwise it carries a reference to the generic.. Deleting first forces the instance to be stand-alone.
For the life of me I can't understand how PTC creo/proe etc etc can be so bad! I thought PTC was one of the pioneers of 3-d parametric modeling/drawing etc ..... They have really dropped the ball; this program is so much more difficult to get anything done .... Solidworks is much easier. I am being forced to use Creo2 now so I read these PTC forums and I keep seeing things like " if you want to get that done you need to stick your elbow in your ear and place your knee behind your back and then do these mouse clicks etc etc" and hope it works; and it might not work this way if you are using windchill etc etc" ..... it's so frustrating
Then go work for a company that uses SolidWorks.
Much of the time it's simply down to the fact that people are too lazy to sit down and learn a topic. Instead they just waste this community's time asking trivial, unintelligent, poorly defined questions. It's often very obvious these people put in very little, or no effort at all, expect others to provide all the answers and give nothing, or very little back to the community.
On many occasions the kindness and efforts of those members who make a positive contribution and continually strive to help people learn is not even acknowledged.
So stop complaining and get to work! You can do that, can't you?
If you put in more effort yourselves, other members would be more inclined to help you when you need help. You might even find yourself in a position where you could help someone else one day.
I apologize if I offended anyone .... I agree with you about putting in effort to learn and also appreciate people's effort to help. But, at the same time, if PTC (and community) only receives positive feedback they will never bother to try and improve their product; and most folks who have used both Creo and Solidworks tend to agree that Solidworks is easier to use and easier to deal with as a company. So again, I apologize if my "poorly defined question" about replacing assembly items without having to change/update references was a waste of time.
You had no question, you posted this review of Creo on someone else's question
Your post was simply a bash about how bad Creo was and how awesome solidworks was.
Creo takes effort to learn. It is NOT Solidworks. Anyone who tries to use it like solidworks will suffer until they quit using it.
I'll admit the responses to your post was harsh but in their defense, your post set the tone.
Again, I apologize .... I thought I was replying on a post that I originally raised a question for last week .... "replacing models without screwing up constraints and references" ..... a question that I actually gave a "kudos" to you SteveWilliams for your answer .... thank you. In my defense I am a 15year user of Solidworks whose company was bought out and new owners are making us use Creo2/Windchill PDM without any proper training; so it is very frustrating. Does not excuse me from ranting on this forum, for that again, I apologize.
I had spoken to PTC directly at a previous job a few yr ago when they 1st rolled out Creo 1.0, we brought up a few issues regarding drawings and this was one of them, i saw very little change in Creo 2.0. For the past year I was on SolidWorks but I am back home in Creo 3.0 M070. I am currently in the same predicament as i need to replace a model bc i need to prototype it and they need drawings so i want to use an old release drawing. I found this video from PTC, but it doesn't have the release or date code. Anyone has a clue what is going on? because this is exactly what we all need. In the mean time i'll go back to coping the old drawing and part, renaming them, copy or model features and add a few dimension in drawing...
FYI, this is Creo 4.0 You can see the same video and additional information in the help documentation:
I just had a similar problem with a part / drawing. I created abs_bracket_2.prt and ended up with a drawing abs_bracket_02.drw. PLM system already had a drawing with abs_bracket_2.drw but I was in a hurry and decided to move on. Created views, dimensions, and then needed to replace abs_bracket_2.prt with a new version abs_bracket_02.prt. Here's how I did it:
Opened original abs_bracket_2.prt, created a family table and a new instance named abs_bracket_02.prt. Opened drawing and used drawing model> replace and then chose abs_bracket_02.prt as it was now part of a family table.
All dims and views stayed perfectly. Save the drawing at this point. Now go back into abs_bracket_2.prt and delete the family table. This will cause family table instance abs_bracket_02.prt to become its own part, no longer an instance. Now open and save abs_bracket_02.prt. Tada!
Honestly, this is just further evidence what absolute garbage creo is.
This should be a simple operation easy to understand and complete. It certainly is in competing CAD programs. Instead, its stupidly difficult and needs a 3 page forum topic to discuss. I still can't make it work. The only possible way CREO users can like this program is if they have no idea how much easier it is out there.
Do you have a specific question? Exactly what do you want to do.
First time poster, new user to the community and no question!
Let me ask some questions.
What version and build of Creo are you using? An answer may vary depending on the version. A bug may be known in some builds by someone here.
How long have you been using Creo?
Did you have formal training in using Creo or Wildfire (though this is out-dated now)?
Why did you hi-jack a thread that was not related to what you posted?
Do you have a real question?
What are you trying to do with replacing a model in a drawing?
Remember, we are all volunteers to this group and can only answer based on what our prior experience has taught us. But, to get a good answer, it requires a good question.
Bashing the software because YOU do not know how to do something and not really asking a question that is easily understood with details as to why you need to do that operation, does not make the volunteers want to answer you.
Please try again in a new message to state what you want to do, why you want to do it and what is preventing you from getting the results you want.