.idw model shows grey lines and I cannot pull dimensions

[ryan]

I am working in Inventor Pro 2018.  This issue just recently started and I cannot for the life of me figure out how to fix it. 

I have a fairly large model, call it 40' x 25' x 4'.  In my .idw I want to isolate a portion of the model that is 12" x 12" x 12".  Instead of doing section cuts, I do a blow up detail of the front then project, then another blow up detail of the side.  This gives me a nice little cube of the portion I wanted isolated and will give me some nice isometric views. 

The issue I am having now is when I want to dimension the parts of the cut out.  It the part was cut by the detail line, the edges are shown in grey and I cannot click to dimension them.  The only lines I can dimension are in black and are edges that are within the 12" cube.  Since the detail cut edges are grey I cannot dimension material thickness since it was cut. 

I have figured out that switching the detail into Raster View will turn the grey lines black and I can dimension them but then I need to switch back before printing to PDF which becomes a big hassle.  I have been using 2018 since Aug 2017 and this was never an issue until March 19, 2018.  Any Idea on how to change my settings???

below is a screen shot of a part to show the line differences and how I cannot select themLines are Grey and Cannot be SelectedLines are Black in Raster View only

[ryan]

Here is another image of the same issue, I can only select the vertical lines which do not help

[Anonymous]

HI @ryan

I have just had a play with inventor to try and re-create your situation.

What i am finding is similar to what you describe. From what i understand the lines that you are trying to select to dimension from are not actually physical edges of the part. The lines that you cannot select are the edges generated by the detail view boundary. These lines belong to the detail boundary and not the part which is why you cannot dimension from them. 

Does this make sense?

Cheers

Callum 

[Anonymous]

I cannot reproduce this, can you upload the model and drawing?

[rayessle]

Using the detail tool is a bad idea for this as you cannot constrain the edge of the detail box to the centre of the hole so you cannot guarantee the dimension being correct to the cut lines. Best to take a section view through the hole, place the view off the drawing then project the required iso view from this new view. this projected view of the cut part will allow you to dimension the cut edges.

You then put the section mark on a no print or off layer so it doesn't show up on the drawing. Alternatively switch off the "definition in base view" option in the view display options for the new section.

Ray

[johnsonshiue]

Hi Guys,

I am confused. Like John indicated here, I cannot reproduce the behavior either. Could somebody share reproducible steps or files?

Many thanks!

[ryan]

Ray,

I understand the constraining portion of it which is what I would do if wanting to pull the dim for the hole.  my question would have been for the glass, it doesn't matter where or how I cut the detail the overall material thickness would remain the same and I cannot select it without going into raster view.

So I created a random part HSS and opened it in the standard mm .idw template, not my custom template to see if I made a mistake.  The line colour is no longer grey (its black) but I cannot select it to put a dim unless I section cut it first.

[johnsonshiue]

Hi Ryan,

Many thanks for sharing the files! You are trying to create dimensions on the detail view, right?  It seems to work fine for me on 2018.2.3. I notice you are still on 2018 RTM. Could you install 2018.2 update followed by 2018.2.3 update?

Thanks again!

[rayessle]

Johnson,

He is trying to put the dimensions on the iso view. See the second image in his first post. He managed to put the dimensions on the second image by changing the view to a raster view.

You were able to select the edges in Inventor 2017, but this doesn't work now in Inventor 2018, when using the detail view to project the iso view. It does work if you use a section that is projected to an iso view.

Ray

[rayessle]

Same part modeled in 2017 & 2018. The 2017 drawing will let you pick the 'cut' edges to dimension, the 2018 drawing will not.

Ray

[johnsonshiue]

Hi! Indeed, this is a change in behavior. I cannot find a good explanation but I am able to reproduce it easily with projected detailed view. The interesting thing is that the 2017 view remains to work fine in 2018. The detail cut edges are still selectable. I will work with the project team to understand the behavior better.

Many thanks!

[andrew_faix]

Hi everyone,

Effectively, @ryan, you were exploiting a defect prior to 2018.  As others have already suggested, the detail cut edge isn't real and more importantly, its position (and shape!) can't be insured due to the nature of how detail views are created (unconstrained).

I was able to replicate the results I *think* you're looking for using a section view instead.  With a section view, you CAN constrain to view geometry (center of the hole in this case).  Moreover, I think this is just better drafting practice in general.

 

Is this good enough?  I really can't justify going back and allowing users to use edges generated by detail cuts.  I don't really understand the point you made regarding a glass part.

[rayessle]

As a by product of not being able to select these edges we cannot switch visibility off for them.

The firs two images below are from Inventor 2017. As you can see we can switch off the visibility of the confusing lines generated from the detail boundary which are not real edges.

The third image is from Inventor 2018. We cannot select the edges so are unable to switch the visibility off. I think that this makes the section view confusing.

Ray Esslemont

[johnsonshiue]

Hi Ray,

Like Andrew explained earlier, the detail view boundary was not supposed to be selectable for dimensioning. It is just a boundary. In 2017 and earlier, it was allowed and it was a bug. To dimension the edges properly, you need to create section views instead.

Many thanks!

[rayessle]

Johnson,

My last post was about being able to switch off the visibility of the lines, not dimensioning. Using a detail view is usually used where you need to scale up a detail because there is not enough room on the original view to be able to document clearly or place section lines. The examples I gave in the screengrabs are simplistic to get the point across. I agree that on these examples I could have taken a section straight from the main view as the difference in scale between the main view and detail view is negligible. In reality it would be more usual to take a detail view to increase the scale/legibility of the view then take sections off of this detail view where we can then place dimensions, notes etc. Not being able to switch off visibility of the detail edge lines can, in some circumstances, make these views more confusing.

Ray Esslemont

[andrew_faix]

Hi Rayn, thanks for the extra details.

I appreciate simplistic examples, but I think we're in fringe territory here.  You're detailing other possible problems that might be revealed as a result of our recent change regarding cut edge selection, rather than practical examples of problems.  We have to be able to differentiate real problems from potential ones.

Behaviors with respect to view geometry and annotation are typically guided by drafting standards, but once you start talking about child views of cut views and isometric view dimensioning, there's little-to-no standards governance here.

WRT to the example you just posted, you generated an auxiliary view from a detail view, and we just don't typically see this behavior.  I agree that in this case, the extra lines created as a result of the detail view operation would be problematic, but it's not clear to me why it would be necessary (from a print-reading standpoint) to create such a view.  If this is common practice, there are other ways to manage the visibility of those edges.  When this particular need arises in your documentation practices, would it be acceptable (as an alternative) to use the "Smooth cutout shape" option" on the detail view?

Thanks again, Ryan.  I appreciate you helping us understand this workflow.  

[rayessle]

Yes, I believe that 'fixing' the edge of the detail view to not allow dimensioning has also made all these lines unselectable for other purposes.

You cannot attach balloons or annotations to these edges. You cannot individually change colour or linetypes of these lines and you cannot switch off the visiblity of them. I do believe that taking a section from a detail view is a common occurrence and I would like to be able to toggle the visibility of these lines to make my views clearer. I understand that there are work arounds and different workflows to try and achieve this, but I these take me more time now than in previous versions of Inventor.

Ray Esslemont

[rayessle]

Here is a less simplistic (real job) example of sections being taken from detail views.

and here highlighted in red  are the lines I hid for section AH. All the lower horizontal lines are created by the detail view edges. The one in the middle of the view is where the section 'steps'. I also did this for all the other sections on this sheet.

Ray Esslemont

[andrew_faix]

@rayessle

OK Ray, I'm sold on the "select-to-control-visibility-and-formatting" issue.  We've got a defect logged on that and should be able to have a fix available directly.

I'm*still* not convinced these edges should be available for annotation attachment.  My main concern here is the volitivity of these edges that could be re-computed by action taken in the drawing rather than the model.  

I appreciate everyone's input on this topic, thank you.

[rayessle]

Thank You.

Ray Esslemont