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RyanBotha
Posts: 98
Registered: ‎01-15-2007
Message 1 of 6 (3,383 Views)

Inventor Drawings. Little annoyances throughout Inventor's life

3383 Views, 5 Replies
07-12-2011 07:31 AM

Hello Community!


I've been using Inventor for a long time now, mainly 3D components with very basic 2D. Recently I was part of a team that had to produce full workshop drawings for a very large piece of equipment (around 510  tons). During the year long project, we found many little annoyances in IDW's, and I'm hoping to remember some of them, so you clever people out there may be able to assist in some quality workarounds.  :smileywink:


For reference; working on T3500 Dell workstation, Inventor 2012 (PDSP)


(Q1) See Image 1. Simple assembly of plates, with chamfer preps for welding. Sometimes we don't want to clutter the view with these lines, but still need them for a scrap detail of the weld. I know we can turn off edges, but that sometimes leaves 'open' edges.


(Q2) See Image 2. I've create a section to reveal the detail of the chamfers, and specify the weld. The section may be mistaken for another complete view (perhaps flatbar or similar), as there are no spline/break lines indicating that the part continues. (See Image 3 for desired view. I know this is possible with a crop over the section view, but if that section view moves, and the crop has not been constrained 100%, the view often disappears, as the crop now removes all detail).


(Q3) Also, the base view is at scale 1:10. The section gets created at 1:10, and after I change it to 1:1, the view shifts up, and the label drops right down. I then have to break alignment, and reposition all elements.


(Q4) Another example that exposes an issue is the section through a flange. In the past, we could use 'draughtsman's license' to depict views, and clearly show component manufacture dimensions. However, 3D is, at times, too perfect. Crazy comment, I know. Let me explain with pictures. Our flanges always straddle centrelines, so when we section through to reveal the flange bolt holes, etc, we have to 'cheat' by creating 2 sections; 1 for the resulting view (B-B) and another for base view definition (C-C). We then turn off the section line for view B-B, and rename Section C-C to B-B, so that the view labels tie up.

 

See Image 4. This may be a silly problem, but I believe it consumes many hours for many draughtsman. View B-B may be an acceptable section for this component, but in many cases it does not work out. We resort to manually  sketching the bolt holes on the resulting section view. Once again, crazy!


So if you would perhaps do two things for me. 1. Tell me I'm not alone! It feels better that way :smileyhappy:. 2. Let me know if you've got any suggestions; they would be greatly appreciated.


Kind Regards,

Ryan

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JDMather
Posts: 26,161
Registered: ‎04-20-2006
Message 2 of 6 (3,377 Views)

Re: Inventor Drawings. Little annoyances throughout Inventor's life

07-12-2011 07:41 AM in reply to: RyanBotha

RyanBotha wrote:

.....We resort to manually  sketching the bolt holes on the resulting section view. Once again, crazy!



Kind Regards,

Ryan



I have had some of my most resistant users completely avoid Inventor (in favor of staying with AutoCAD) because Inventor doesn't do everything for them.
Not to discount anything you listed that Inventor should do for you, I see nothing wrong or abnormal with manual editing of views as needed to depict design intent.  I can't understand the AutoCAD users who refuse to manually edit an Inventor view but go back to AutoCAD and do everything manually.  That is crazy!

 

Be sure to submit to the Autodesk wishlist and participate in Beta.

 

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Valued Contributor
RyanBotha
Posts: 98
Registered: ‎01-15-2007
Message 3 of 6 (3,335 Views)

Re: Inventor Drawings. Little annoyances throughout Inventor's life

07-12-2011 08:37 AM in reply to: JDMather

Agreed! No doubt, I fully appreciate what you're saying. I used to work at a reseller, so I've had many years 'converting' people. However, when manually editing views in Inventor, the drawings become SO fragile, as to make me too scared to open them after a small change to components. Every had Inventor vomit pink everywhere, especially after a small design change. Co'mmn JD, don't tell me that doesn't get under your skin.

 

Second, these problems are the ones that continue to bug me/us, until eventually your sanity gives way, and you start slapping the monitor. I've never allowed anyone to 'opt out' though, and head back to CAD. We stick it through, and finish in Inventor, however painful.

ron
Member
ron
Posts: 5
Registered: ‎01-31-2007
Message 4 of 6 (3,295 Views)

Re: Inventor Drawings. Little annoyances throughout Inventor's life

07-12-2011 10:53 AM in reply to: RyanBotha

(A1)  Did you know that you can select the extra chamfer lines and RMB select "Visible" so they won't display?

 

(A2)  I would create a side view (the chamfers would still be visible), then pull out a Detail view.  If the chamfers are not visible in the side view, then make a break-out and detail that.

 

(A3)  See above.

 

(A4)  I think you are doing this all wrong.  First, DO NOT ADD GEOMETRY MANUALLY  - it's error prone and can get expensive if your parts are made incorrectly.   Did you know that you can create a section which goes from the top "B" down to the center of the flange, then down to the "6-o'clock" position where the lower "C" is shown?  This would be the correct way to depict this IMHO. 

*Expert Elite*
dan_inv09
Posts: 2,297
Registered: ‎12-12-2006
Message 5 of 6 (3,258 Views)

Re: Inventor Drawings. Little annoyances throughout Inventor's life

07-12-2011 01:33 PM in reply to: ron
RyanBotha "I know we can turn off edges, but that sometimes leaves 'open' edges."
 
ron "(A1)  Did you know that you can select the extra chamfer lines and RMB select "Visible" so they won't display?"
 
if I'm not mistaken: RMB select "Visible" = turn off edges
 
Anyway:
Are the chamfers in prep and the holes in machining in your weldment? (If you dill the holes in the part you can turn off the prep in the view. (Of course then your section has to come from a different base view, doesn't it?))
 
I always turn off the lines on the "ends" - of course for seemingly no reason at all they come back once in a while.
 
The views are probably still as in line as they were before but if the center of the section was 1/2" away from the center of the other view now its going to be 5" away - Is this what "View Justification" on the "Display Options" tab is supposed affect? (I know the Help was bad before but this wiki thing ...)
And the label is probably also the same relative distance from the center - you could change the scale while placing the section view rather than doing that later.
 
I would run the section down the middle to the center and then angle it so it goes through one of the holes. Now, I've got parts with several hole patterns - I can get two in the section that way, but I'd like to be able to get them all.
 
Autodesk was always very fond of saying that they followed standards when setting all this stuff up and at their little roll out functions there was always someone who would say "Do you want me to get my Drafting book?" (You'd think they'd know not to invite current users.) One time someone had a copy with them, it was a different edition than the ones I had but it still had the same examples - how to section with ribs or spokes,etc. (and hatching should not be at the same angle as lines in a view - like it is in your countersink detail, tsk tsk) - that was usually when it suddenly became time to award some door prize or something.
Valued Contributor
RyanBotha
Posts: 98
Registered: ‎01-15-2007
Message 6 of 6 (3,208 Views)

Re: Inventor Drawings. Little annoyances throughout Inventor's life

07-13-2011 12:48 AM in reply to: dan_inv09

@ron - Did you know that you can select the extra chamfer lines and RMB select "Visible" so they won't display?

 

(A1)  Yes, thanks. I did.

 

(A2) That is another option I had'nt thought about yet. Seems long, but if its rock solid during part changes, then its worth the extra view creation. I'm not too sure how robust the break-out view is. Probably also requires constraining of the sketch.

 

(A4) Seems like a good option. Thanks.

 

@dan_inv09 -  Is this what "View Justification" on the "Display Options" tab is supposed affect?

It does in some ways. After having sketches shift around over the views, especially if they're not dimensioned, I always place views with the 'Fixed' option enabled. 

 

@dan_inv09 - (and hatching should not be at the same angle as lines in a view - like it is in your countersink detail, tsk tsk)

Yeah, whoops! Copied off an old AutoCAD drawing. :smileyvery-happy:

 

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