As I sit here in my Creo training class, making a drawing, I create an auxiliary view, no problem. I'd REALLY like to crop that view... and I'm at a road block. I've typed 'creo crop view' in the forum search, and checked my book index. I just can't seem to find anything related to cropping a view in Creo. What am I missing?
I have gone back to my model, looking for somethign to do there (like I need to do for a section View), but again... I'm stuck. A little help please...
If I can't crop a view, please just give me the painful news quickly Thanks!
Solved! Go to Solution.
Sorry to hear that you are suffering thru training!!!!
In Creo Parametric to "crop a view" as you are calling it, select the veiw, right clich and hold, select properties, change to "Visible Area".
Select one of the options from the drop down menu (default is "Full View"). Depending on your choise you will need to tell Creo how you want that option defined.
Since you are in class, play around a little and you will see that the definations are pretty easy!
Thanks Stephen & Kevin! I knew there had to be an easy way. Everything seems to be 2-3 layers deep in Creo, I'll get there eventually.
As a clarification for future seekers:
RMB View Propeties / Visible Area / View Visibility pull-down / Partial View
Click the model somewhere in the area to be kept, sketch a spline boundary.
Show/hide the crop boundary, Apply, OK.
When you pick a place - choose carefully.
It is a point on geometry to anchor the boundary. If that geometry changes, the point may be lost or move, leaving the boundary that is defined relative to that point to float.
Thanks David, very good note & a lesson we've all learned at some point! Generally, the only drawing view items I will tie to a model are section lines and aux view definitions. Even then, I tend to use datums (reference geometry in SW) such as planes & axis. It's no fun when your drawing views go wonky because of a model change!!
In anyone is having a problem with model entities being auto selected when defining a view, go into your settings and turn off the auto-select. After your dwg views are defined, turn them back on for dimensioning, etc.