Unacceptable... Having to fix IDWs nearly every time I open them.

[Anonymous]

I have had to "fix" several IDWs multiple times, causing me to lose hours of work time. This is unacceptable and I need to resolve it now.

What I mean by "fix", is, when I open an IDW file that was previously created and has had a part added or modified, the entire drawing becomes jumbled... Bubbles lose alignment and some lose attachment to parts, Detail positions are moved, Detail boundaries are not located where they were placed, parts are turned off... seriously... there's no nice way to put this, WTF is going on?? I know this can not be normal, but it has happened to me about 5 times and I've literally lost hours and hours just "fixing" something that should not need fixed.

I am attaching a png file to show what I mean. This file was pristine when I last saved it, complete and ready to give to the shop. I had to change part #15's length. I did, and fixed iProperties description, then reopened the IDW, and what you see is what I get....

Details A and B:

bubbles are not aligned with each other anymore.

Some bubbles are not even pointing to anything now.

Both detail boundaries has moved from their original locations on the assembly and no longer display the correct area of detail.

The details themselves have moved... Detail A moved to the right, too close to the assembly, and Detail B moved to the left, too close to the edge of the paper.

I really can't be spending hours a day correcting files that magically change themselves.... please help!

[LT.Rusty]

Couple things.

1.  Not sure how you expect things to not change when you change something.

2.  Try attaching the details to a reference point that.  When that reference point moves, the detail will move as well.  If, for instance, you had attached Detail B to a reference point - say one of the flange bolts, for instance - then when the length changed, the whole detail view would move as well.

[blair]

Or just select the "Defer Updates" and then you can make all the changes you want to the model and the drawing won't update until you request it.

[Anonymous]

1. What I expect is that, by lengthening one pipe (#15 in detail A) by 1/2"... the entirety of the IDW file should not lose its marbles. There should be literally no effect on Detail B... and Detail A could easily encompass the change without any moving of bubbles, turning off of parts, moving of detail boundaries, detail being moved.

2. What do you mean by attaching Detail B to a reference point? Are you saying that the center point of the detail boundary can be constrained to a specific point of the assembly geometry? Even if that is the case, I don't want the details to move around the sheet.

[Anonymous]

I'm not sure that this is a solution to the randomness of everything moving on the sheet. However, I will keep this under advisement for my future IDW files. Thank you.

[brendan.henderson]

Here is a good article about attaching details to views.

http://blogs.rand.com/manufacturing/2013/01/attachment-to-detail-its-the-little-things.html

[SBix26]

Along with the other suggestions for keeping the details reliably located, make sure the base view justification is set to Fixed instead of the default Centered (Edit View > Display Options tab > View Justification).  This makes it less likely that the view will move when components are added, modified or deleted, thereby changing the view envelope.  I assume that the fixed point of the view is the assembly/part origin, but I haven't tested that assumption.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
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[swhite]

This is beacuse if you add a part, the view tries to make room for that added part, even if it means having to shift positions. Sometimes merely repositioning your original detail circle will fix the issue. The only sure fix is to create view reps of what you want to see in each view and lock them. This prevents new parts from showing in the view rep, so if the part needs to show you will have to unlock the view rep and update. But of course that leads back to your original problem. You can hide the new part and your view will go back to its normal position, it all depends on if that part is needed in the view. The only part that really bothers me is if a view is cropped and a part added, it shows it anyways even if outside the original cropped area, causing everything to shift. It is simple to hide the part and the view will reset, but if outside the crop area, it should never show in the first place IMO. Otherwise why bother to crop a view?

try repositioning your orignal A and B view detail circles first.

Its only too bad you cant set a point in a sketch on the drawing and create a detail view centerd on it, similar to skecthing a line and using it to create a section view.

[Anonymous]

I appreciate you posting this link... I didn't understand what was being suggested by LT.Rusty earlier, but now I do, and I will assimilate that into my workflow. Thank you.

[Anonymous]

Also added to my workflow. =D thanks!

[Anonymous]

I think this is the answer I was looking for. It explains why things jumped around on the page... utilizing this information and tips for fixing the issue, along with fixing the justification of views, attaching detail boundaries to geometry, and potentially deferring updates (haven't tried this yet...), I believe may solve many of the issues I'm seeing.

I am currently creating Design Views, but I don't see a lock option anywhere.... where is this option?

*EDIT* Nevermind, I found the option, which was as simple as right clicking in representations in the browser bar. Thank you for your help =D

[BLHDrafting]

Assimilate! Are you a Borg JWittACS?

[Anonymous]

Yes, however a grammatical error in your logic needs to be rectified... WE are Borg. 

"Assimilate: Take in (information, ideas, or culture) and understand fully." ~Google

[BLHDrafting]

Grammar error proves I AM NOT BORG! Cheers