Drawing views shifting when model changes

[BPapp]

Running Creo 3.0, build M020 with Wildfire.

We do large aircraft assembly and modification models and drawings. What happens is we can complete a model and then complete the drawing. If anything changes on the model it can cause views on the drawing to move. In the past we were careful to compartmentalize drawings and models in unique stand alone directories. With Windchill that is no longer possible.

What I am faced with is I spent close to 100 hours doing a complicated drawing with lots of fasteners depicted by symbols.

I completed the drawing and checked it in. Recently I went back just to review something and every view is scattered, because work had continued on the master model. Livid doesn't begin to describe how I feel. It happens to everyone in the group. Locking View movement doesn't stop  it. Associating draft entities doesn't help. I was even told to put a blank view off the format and erase it, then it wouldn't happen.

Is there something really simple we missing to prevent this?

It's not practical to wait until the master is fully complete to start drawings. There are way too many subsystems going on.

Hopefully the description of the condition is clear and others have experienced it, and found a solution.

Windchill has really aggravated the issue, because we now have to all use one model.

Thanks for any help with this issue.

Bruce

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[slapha]

We've had this happen too, especially on a revision where someone starts updating the model and goes to update the drawing later. We're on Creo 2.0 but the change is the same. Basically the views stretch to match the model.

I’ve found the following

• View associated symbols, and dimensions will scale relative to the overall size of the view, even if those individual features didn’t change
• Views will adjust so that the center point is still at the center of the original view, this includes some changes to the skeletons  (if you're using view center as origin)
• Non-associated symbols or annotations will remain in the location that they were placed (though everything around them could change)
• Datum features on a skeleton will not update view size
• Shapes and sketches on a skeleton will update a view size even if not visible

I even made the following and show some examples of what I found

https://community.ptc.com/t5/Creo-Parametric-Ideas/Add-a-way-to-prevent-views-from-moving-after-changes/idi-p/468637

The response was in short make partial views and relate the view origin to something that won't change, like CS0.

Also check for exploded view, for some reason that got turned on by default in some of our models/views.

[mender · Accepted solution]

If the views are *shifting*, then it seems likely that they are using the view center as the origin.  If you expect you may be making changes that affect the view outline, using stable geometry (usually the assembly's base csys, perhaps via drawing_view_origin_csys) as the view origin is a good plan.

This won't address issues of certain detailing items parameterized relative to the view outline having this placement move when the view outline changes, but it's a start.   Addressing that would involve a rather substantial project, which has for a number of releases not made the cut.

[BPapp]

Thanks Matthew. I appreciate your honest and helpful response. I'll try that, and hopefully that helps some.

Bruce

[dschenken]

Since the view-related draft items have locations scaled according to the view boundary, if the visible portion of the items does not change apparent size, one can set views to be Partial views and draw the boundary as desired. This will fix the view boundary and with it the size of the view, etc.