12 Replies Latest reply on Mar 16, 2016 3:56 AM by Greg Hynd

Using section view made in assembly in a drawing?

Richard Yang Mar 14, 2016 5:16 PM

Hi there,

I made a section view in a Solidworks assembly that shows only the front portion of a design, so that everything behind it doesn't show and confuse the viewer (since the front object has holes). When I tried to move it over to a drawing, the sectioned portion would be deleted, and go back to showing what used to be behind the object. Is there any way to have views in a Solidwork drawing where I can basically hide anything behind a certain plane?

For example.

Object 1 Object 2

{} [====]

From the left hand view, I should only see {} from that side, not anything from object 2. This is easy in a section view in an assembly, since I can just make a section view to cut in between the two objects, and then set my orientation to left hand side to see that side of object 1 without anything from object 2 showing from behind. I can't seem to move that over to a drawing after i've saved the section view, nor can I replicate something similar in a drawing. Section views in drawings don't do what I want either from my current knowledge, since it would give me the view from in between object 1 and 2 if I cut in between.

Is there anything I can do to only display the front most objects in a view and hide anything behind it? Let me know if I need to include more information to make this question more clear.

Cheers!

--------------------------

EDIT

To clarify what I am asking, see the example I have created below. This is the isometric display for the 2 "levels" of objects in my design. I want to be able to create a front view in my drawing where I only see the objects in level A, so basically nothing from panel B will be showing and confuse viewers.

In the assembly this is easy, I just make a section view and set the plane to somewhere between the two levels.

Click "OK", change my orientation to front, and voila, all I see is a front side view of level A.

How can I do this in drawings?

Cheers,

NOTE: Also note that I would like to do the same for the left hand view. Same idea applies, only I would like a left hand view with only the front most item showing.

Re: HiUsing section view made in assembly in a drawing?

Jacob Ames Mar 14, 2016 5:02 PM (in response to Richard Yang)

Hi Richard!

Once you've placed your section view in the drawing, try using the Slice Section option in the property manager. I think this will address the problem you're having without any difficult workarounds. Let me know if this works for you!

Regards,

Jacob
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- Re: Using section view made in assembly in a drawing?
  
  Richard Yang Mar 14, 2016 5:12 PM (in response to Jacob Ames)
  
  If it is easier, please see the edit to my original question for more clarification. When I try to place the section view in the drawing, it automatically deletes the section and just shows the whole assembly automatically. Will the slice section keep the section view intact? I will give it a go.
  
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Re: Using section view made in assembly in a drawing?

Jeremy Feist Mar 14, 2016 5:09 PM (in response to Richard Yang)

I would recommend using display states instead of section views. you can set your projected views to show a particular display state ( like one that only shows object 1).

if you are set on using a section view created in the model - you need bring in the correct parent view - I do not know how to control which view SW chooses for the parent for the section.
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- Re: Using section view made in assembly in a drawing?
  
  Richard Yang Mar 14, 2016 5:11 PM (in response to Jeremy Feist)
  
  If it is easier, please see the edit to my original question for more clarification. How can I get my display states to show only one side of a chosen plane in an assembly? I know that you can choose specific items to hide, show, etc, but I want it to show everything on one side of a plane (includes small parts and pieces of some bodies).
  
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  - Re: Using section view made in assembly in a drawing?
    
    Jeremy Feist Mar 14, 2016 5:42 PM (in response to Richard Yang)
    
    the simplest way to create a display state is to select everything you want to show, (sounds like a box select from the top view would work for your specific application) right click and choose isolate. this brings up a flying toolbar with a save button on it. hit the save button, and give the display state a name.
    
    you can also box select everything you wish to hide, invert the selection, and then isolate.
    
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    - Re: Using section view made in assembly in a drawing?
      
      Richard Yang Mar 15, 2016 7:15 AM (in response to Jeremy Feist)
      
      Would this allow me to select a section of a part to include in a display state?
      
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      - Re: Using section view made in assembly in a drawing?
        
        Fred Zobel Mar 15, 2016 4:54 PM (in response to Richard Yang)
        
        Display states will not show you a section view of a part. Parts are either there, or not there when hiding them.
        
        As far as sections. If you create a section in a model, you can bring them in to your drawing and show them as long as you save them as an annotation view in the model. This does require having a parent view that can show the section line, and you can't really get isometric sections this way.
        
        You can create isometric sections by adding a configuration with an assembly feature cut that cuts away parts and sections of parts and show that configuration is an isometric view.
        
        Based on your simplified example, a display state would be the way to go.
        
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      - Re: Using section view made in assembly in a drawing?
        
        Jeremy Feist Mar 15, 2016 10:07 AM (in response to Richard Yang)
        
        no it will not.
        
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Re: Using section view made in assembly in a drawing?

Greg Hynd Mar 15, 2016 10:13 AM (in response to Richard Yang)

Richard,

In the drawing sheet, create a section using the section line tool. In the section view property manager you will see an option for section depth, select this, drag the red line to the depth you want to show, and you will achieve the result you want.
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Re: Using section view made in assembly in a drawing?

Richard Yang Mar 15, 2016 1:50 PM (in response to Richard Yang)

Greg offered the best piece of advice for doing what I asked, using the section tool and then providing the depth. However, I could not find a way to get rid of the section line that showed where it cut. I used another way that provides a bit more customization, although it is not as nice of a solution.

I just ended up making a bunch of different configurations for each cut that I wanted, and made an extruded cut to hide the components that I didn't want to see. This was beneficial since I could cut shapes that were not restricted to just planes. I then just use the center, LH, RH, and top views of that configuration in my drawing to show the viewpoint that I wanted, displaying only the items that I wanted.
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- Re: Using section view made in assembly in a drawing?
  
  Greg Hynd Mar 15, 2016 4:40 PM (in response to Richard Yang)
  
  Richard,
  
  Not in front of solidworks now but I believe you can right click your section line and hide it in your drawing. Will check in the morning.
  
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  - Re: Using section view made in assembly in a drawing?
    
    Greg Hynd Mar 16, 2016 3:56 AM (in response to Greg Hynd)
    
    See picture. hopefully this helps.
    
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