i have created a drawing file(drw_1) and made copy of the file(drw_2) in same folder if i delete any of the dimesion or view in the copied file(ie., drw_2) creo automatically deletes the same in the source file(drw_1) is there any solution for this issue if so let me know that.
I guess both drawing have the same drawing model assigned. Therefore dimensions can disappear. I do not know why views are missing ...
I am facing the same issue but here it is not related to the dimension. I have deleted or created annotation in the new drawing and the same has been reflected in the old drawing as well. do you have any thoughts about this.
I was creating a revision drawing So both drawing shouldn't be the same.
Thanks in advance.
If you make your dimensions with 'create_drawing_dims_only yes', then they will be made in the drawing, as opposed to being made in the solid. A drawing made in this way will not exhibit this issue.
More specifically to what Matt wrote - don't delete these dimensions from the drawing, use Erase.
The dimensions were created in the drawing but with the Configuration setting so that the created dimensions are stored in the model. Ordinarily this isn't noticed because people who Create dimensions would not Show the draft dimensions on other drawings. Because this is a Save-As of the drawing alone, the same model is used in both drawings and the same dimensions (carried in the model) are Shown in the drawings. Deleting a Created dimension stored in the model that is Shown in the drawing deletes the dimension from the Model.
The best approach is to Show dimensions from the Model and never Create drawing dimensions, but PTC hasn't covered the failure mode in Shown dimensions that makes Created Drawing dimensions prized - if a feature is redefined or deleted and replaced, the drawing will not echo the deleted Shown Model dimension, prompting the drafter to fix/account for the change. At least with Created Drawing dimensions the dimension and leaders will remain and change color to show their broken status.
The setting Matt mentions is also useful when the Part/Assembly is Released/Checked-out by someone else/otherwise Locked (That was a nice feature in PTC Intralink that didn't make it to WC Intralink) to prevent the part being changed by the Drawing Mode Created Dimensions being stored in the related Part/Assembly.
One clue to this is that there could have been a prompt that the model was being modified by deleting the dimension, just like there should have been a prompt that the model was being modified when the dimension was Created.
-thanks for your response Mr. David schenken.
As u said instead of deleting the dimension we can erase, "for dimension erase suits but in case where we have to delete a view we can't use the erase if so we can't delete the model from model properties and the model will be carried where ever we move the drawing file."