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visibility in 2d drawings

16 REPLIES 16
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Message 1 of 17
hoaglin14
1764 Views, 16 Replies

visibility in 2d drawings

This is probably a question with a simple answer that I haven't found the answer to.  I want to be able to hide a part of an assembly in one projected view of the 2d drawing but not all, however when I do so the hidden lines stay hidden lines. They do not change. I know you can change the hidden line properties to make them continuous lines but is there a setting that will allow these lines to change automatically?

16 REPLIES 16
Message 2 of 17
mcgyvr
in reply to: hoaglin14

umm..something else must be wrong. When you remove the visibilty of a part that was over other parts the hidden lines will change to continuous lines automatically. What version of Inventor are you using?



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Inventor 2023 - Dell Precision 5570

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Message 3 of 17
Yijiang.Cai
in reply to: hoaglin14

Could you attach some images or drawings for more details?

 

Thanks,
River Cai

Thanks,
River Cai

Inventor Quality Assurance Team
Autodesk, Inc.
Email: River-Yijiang.Cai@autodesk.com
Message 4 of 17
hoaglin14
in reply to: hoaglin14

I attached an inventor drawing that has the hidden line problem

Message 5 of 17
johnsonshiue
in reply to: hoaglin14

Hi! Please attach the model file (ipt or iam) too. IDW file is not enough to see the drawing views.

Thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 6 of 17
hoaglin14
in reply to: hoaglin14

Here is the part file

Message 7 of 17
mcgyvr
in reply to: hoaglin14

hoaglin,

1 part and 1 idw is not enough to show the problem.. You need to attach an iam and all the ipts in that plus the idw and a screen shot would be nice too showing the issue. I suggest you zip up all the parts/iam/idw/screenshot and post that.

 

For your reference an idw (or iam) is simply a file with links/references to all the files in it.. they are not included in the idw (or iam) file itself. So for example if you have a problem with an iam file you need to include that iam file plus all the ipts in it.



-------------------------------------------------------------------------------------------
Inventor 2023 - Dell Precision 5570

Did you find this reply helpful ? If so please use the Accept Solution button below.
Maybe buy me a beer through Venmo @mcgyvr1269
Message 8 of 17
hoaglin14
in reply to: hoaglin14

Hopefully this is everything. I just want to know how to hide a part in a drawing file without leaving hidden lines behind.

Message 9 of 17
Yijiang.Cai
in reply to: hoaglin14

I assumed the original state of base view shows in the attached image.

1. Please right-click the component in browser which you want to hide in the view.

2. Select "Select as Edges" in context menu

3. Right-click the highlight edges in view, select "Visibility"

 

You will see all the project edges from the selected component will be invisible. When the invisible edges are expected to show, please right-click the view then select "Show hidden edges", and right-click the highlight edges in view to select "Show All" in context menu.

 

Thanks,
River Cai

Thanks,
River Cai

Inventor Quality Assurance Team
Autodesk, Inc.
Email: River-Yijiang.Cai@autodesk.com
Message 10 of 17
raymondxu
in reply to: hoaglin14

An easy way to hide a part is,

1. Select the part node on browser under the projected view

2. Uncheck "Visibility"

 

Best Regards,

 



Raymond Xu
Software Architect
Autodesk, Inc.
Message 11 of 17
SKinzel
in reply to: raymondxu

I have an IDW of a weldment that has the "visibility" of objects greyed out.  This is a two piece assembly that is bolted together and I am trying make the bolts invisible in the section view so that the drilled and tapped holes can be seen.  None of the parts in the browser have "visibility" available when I right click on them.  I've done other weldments just like this one (as far as I can tell) and I am able to turn toggle the visibility of the different parts in the views.

 

Is there a setting in the IAM or IDW file that makes "visibility" available?

Stuart Kinzel
Inventor 2013-64bit, HP EliteBook8740w Intel Core i5CPU 2.67 GHz
8GB memory
Windows 7 64bit
Message 12 of 17
SKinzel
in reply to: SKinzel

Okay, I think I found the setting.  I edited the section view and on the Component tab under Representation I changed the View from "Default" to "Master".  This cleared the "Associative" checkbox which lets me then change the visibility of ojects in the view.  I've never played with this setting before so I'm not sure why some of my weldments would be set one way and others set another.

Stuart Kinzel
Inventor 2013-64bit, HP EliteBook8740w Intel Core i5CPU 2.67 GHz
8GB memory
Windows 7 64bit
Message 13 of 17
bobvdd
in reply to: SKinzel

The problem and solution are also explained on our support blog.

Cheers

Bob




Bob Van der Donck


Principal UX designer DMG group
Message 14 of 17
SKinzel
in reply to: bobvdd

If I understand correctly controlling the visibility from the assembly would toggle visibility for all views of that assembly.  My issue was needing to turn off visibility of components in only one view.  I guess I'll need to make sure I manually update if I make any changes.

Stuart Kinzel
Inventor 2013-64bit, HP EliteBook8740w Intel Core i5CPU 2.67 GHz
8GB memory
Windows 7 64bit
Message 15 of 17
bobvdd
in reply to: SKinzel

You can use a different viewrep per view in the drawing. You  could create yourself a viewerp in the assembly that removes the visibility of a particular part and then use that viewrep just in one view but not in the other views.

Bob




Bob Van der Donck


Principal UX designer DMG group
Message 16 of 17
SKinzel
in reply to: raymondxu

The problem is that visibility was not available in that view in this particular drawing.  The only way I could get visibility to be available was to change the associativity of the view.

Stuart Kinzel
Inventor 2013-64bit, HP EliteBook8740w Intel Core i5CPU 2.67 GHz
8GB memory
Windows 7 64bit
Message 17 of 17
SBix26
in reply to: SKinzel

You create view representations as needed in the assembly file (.iam).  Each view in your drawing (.idw), if associative is checked, is controlled by one of those view representations, which you choose in the Edit View dialog box.

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