Section view only for selected parts in an assembly

[Anonymous]

Hi,

Is it possible to define a View Representation in an assembly such that a half section view is active, but only for a certain set of parts within the assembly?

Thanks

Daniel

[alessandro.gasso · Accepted solution]

Hi Daniel,

Please, try the following.

• Edit the part you don’t want to display sectioned in the Representation view within the assembly.
• Menu Tools > Options > Document Settings > Modeling tab.
• Uncheck the box Participate in Assembly and Drawing Sections.

• Return to the main assembly.

I hope you can find it useful.

Kind regards,

Alessandro

[Anonymous]

Hi,

Thanks, it works. A more flexible solution would be maybe a per-assembly solution (a given View Representation within an assembly could be configured to be valid only for a given set of parts).

Daniel

[alessandro.gasso]

Hi Daniel,

I’m glad I could be helpful.

I’m not sure I’ve understood your suggestion, but it seems a bit tricky storing this setting about which part I want to section and which not, in the Representation view if this is what you mean.

Maybe another approach you can use, if you know before creating the parts, which one you want to section in the assemblies and which one not, is to store the setting I’ve suggested in my previous answer in a part template.

Then you can create the parts you don’t want to section in the assembly, from this template.

Of course, if you change your mind for one part after you have created it, you can always change the setting again.

Kind regards,

Alessandro

[aries.1482]

Hi,

I have one part, but in two assemblys: assembly A and assembly B. I want to section the part in assembly A, and not B.  So I must create two copies of part?

Thank you!

[Anonymous]

Hi, does this also work in Inventor 2011?

[Anonymous]

Hello,

I was wondering if this feature is available in Inventor Professional 2016? I cant seem to find that option within the settings. 

Thank you,

Michelle

[Anonymous]

Bump. Anyone know how to do this in 2016? ~Justine

[Anonymous]

I did this to my assembly and it`s working just fine until the moment I want to save it. For example I have a sectioned assembly and I selected which parts not to be sectioned. The representations is ok, but after I save the file and open it again next time all the parts are sectioned including the ones I`ve changed the option "Participate in Assembly and Drawing Section" My question is how to save the sectioned view the way I want it? Thank you.

[Anonymous]

Hi, I have an assembly made of 2 parts (one big and one small) that are made of multiple bodies. 
I want to make a half section and cut the bigger part and move the uncut small part to check the trajectory and interference? 

I did your steps but no success.

Inventor professional 2016

Regards 

Dean

---

@alessandro.gasso wrote:

Hi Daniel,

Please, try the following.

• Edit the part you don’t want to display sectioned in the Representation view within the assembly.
• Menu Tools > Options > Document Settings > Modeling tab.
• Uncheck the box Participate in Assembly and Drawing Sections.

• Return to the main assembly.

I hope you can find it useful.

Kind regards,

Alessandro

---

[Anonymous]

AutoDesk does not "get it"!

Being able to exclude a part from being sectioned in a specific assembly is what is needed. Not every assembly!

By making these setting at the part level (ipt) it excludes sectioning in every assembly! Which is the least flexible condition. The same goes for Phantom and Reference settings for BOM table generation. The part could be Reference in one assembly and Phantom in another, and normal in yet another assembly! And, this is not a unique or rare occurrence. Both SolidWorks and Creo (Pro/E) have done this for years.

[ProKAD]

I've spent over half and hour searching how to exclude a part from a section view in 3D model space, as most of the answer relate to sectioning views in drawings and this is seriously the best solution Autodesk have to offer? Please someone tell me that it's down to my ignorance and not the limitations of the software.

Ps. I seriously miss Solidworks.

[Anonymous]

Yep. I have not found that one either! It's so easy to criticize CAD software. I don't think I'm ever pleased with what I have to work with at time I'm using it.
Inventor has its faults and seems clunky. But, it also does some things really well. Oh well. Continue the fight! Think of it as a challenge.

[Anonymous]

Thanks so much. I've been trying to do this for so long without success.

[Anonymous]

 Just right click on original view and suppress it 

[Anonymous]

But what if I want to see that part in the original view?

[johnsonshiue]

Hi! I just want to clarify a few things. The document setting to control sectioning participation works in model files (iam and ipt) and drawing files (idw and dwg). In the model files, when the setting is checked, the component will be sectioned using Section View command in View tab. In the drawing files, the same setting only control the default behavior of given component in a section drawing view. Whether or not a given component participates in a drawing section view can be controlled in right-click context menu individually. So, you can have a component not sectioned in the model environment but sectioned in the drawing view and vice versa.

Many thanks!

[cvbt-thailand]

To clarify:

In the drawing, in the Browser, Expand the children of the sectioned view

> Right click on the component

> Click on Section Participation

> Select Section to show the part as sectioned,

     Select None to show the part whole (unsectioned).

[Anonymous]

Hello Alessandro,

I am in a beginning Inventor class at De Anza College. 

We are using the text book, by Daniel T. Banach & Travis Jones, "Autodesk Inventor 2018 Essentials Plus".

We are at Chapter 6 of the book on Creating and Documenting Assemblies.

One of our assignment is to work on a presentation file of the assembly.  One of the views required that one particular part be half section by a datum plane, but the rest of the neighboring parts are not sectioned.  Please see attached PDF file, on sheet 3 is the view with the one part sectioned.

I read your suggestion on how to do this.  But, frankly, I have a great deal of difficulty following your three sentences, starting with the very first sentence.  Would you please walk me through what we are supposed to do?  How does one edit the part you don't want to display sectioned?

• Edit the part you don’t want to display sectioned in the Representation view within the assembly.
• Menu Tools > Options > Document Settings > Modeling tab.
• Uncheck the box Participate in Assembly and Drawing Sections.

[johnsonshiue]

Hi! There are two ways to control how a given component display in section view. The process Ale described was specific to document based. It means the sectioning behavior will persist per document. The setting applies to the model section view in assembly and the part, and also the drawing view.

There is another way to control sectioning behavior in drawing view particularly. In a drawing view, if you do not want a given component be sectioned, you can simply right-click on it in the browser -> Section -> None.

Many thanks!