In that case, I have to delete the existing views and create them again, not replacing them with the existing.
Yes I'm quite sure you cannot replace a fully dimensioned drawing view like that.
I think this should be a feature request.
There is a way to do it tho, but it's roundabout.
Save the existing drawing as a new file in a new location. Move the original part (cut and paste) to your desktop. When you open the new drawing, it wi ll try to find the part. Point it to the new part. Then copy new drawing and new part where you want it.
Quite a lot of steps to do something I think we should be able to do in the first place.
Yes, that will only be an alternative to replacing the complete model in the drawing file but not replacing the model from different sheets in the same drawing file.????
Drawing File : ABCD
Sheet 1 : Model A
Sheet 2: Model A
Sheet 3: Model A
Drawing File: ABCD
Sheet 1: Model A
Sheet 2: Model B
Sheet 3: Model C
Try replacing the models by changing references...surely you cannot replace 'models as per sheets' in the same file like references in a 'copied file'..?? any other suggestions??
No. UInfortunately that cannot be done.
The easiest way I have found is to choose the file open option and browse out to the sldrw. Pick the file. Before opening it, choose the references option. double click on the part name of each part in the file and replace the existing file with the new file.
I know you can use the solidworks explorer to replace the models which are referenced in the drawing by going under the references tab once you locate your file in the explorer.
So you could copy your whole file and then replace the references in the new file. You would then have two sheets with different parts but not in the same file. Will solidworks let you copy the sheet over into one of the two files? I've never tried it, but they must have some way to combine sheets from multiple files into one.
Maybe there is some way to do it in the solidworks explorer. It works fairly well from the few times I've had to do it.
There are a couple of ways, teach this to the students.
One is how Paul said above and 2 is when the students don't follow dirrection and did all their work in single drawings.
if you select the view and control C the go to the new drawing and control V it copies the view and the dims....done.
here is a pdf from my class, one drawing file 11 sheets with assembly and parts.
Message was edited by: Lenny Bucholz
name is on there to stop cheaters
TROLLEY ASSEMBLY.PDF 1.8 MB
I'm using SW 2016 here's how:
Key is to use SW explorer.
- Make a duplicate of your original files and hide them under another folder temporarily
- Rename your updated files (part and assembly) with the same name that were used in your drawing using SW explorer.
- Rename only your drawing file using SW explorer.
- Open the drawing using SW explorer - you should see all your parts and assembly updated with the new updates.
- Save your drawing and close.
- Now rename your part and assembly with the new name you want using SW explorer. - this is where SW explorer will do its job.
- Open your drawing now you should see the parts and assembly updated with the new names.
Found a way to replace a part or an assembly in SW2016, but one view at the time... Open your ".drw" file, then go in the FeatureManager Design Tree. When you right click you have an option to "Replace Model". Select that, and you'll be prompted to select the replacing
EDIT: After you get prompted, there is a check box to replace All Views. So you don't have to do one view at the time :-)
Personally I don't think it is a good idea to have different parts in one drawing.
Why don't you create display states or configurations in assembly to achieve your goal on drawings.