AnsweredAssumed Answered

Using section view made in assembly in a drawing?

Question asked by Richard Yang on Mar 14, 2016
Latest reply on Mar 16, 2016 by Greg Hynd

Like • Show 0 Likes0
Comment • 12

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.

Richard Yang Mar 15, 2016 1:50 PM

Correct Answer

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.

See the reply in context

No one else had this question

Outcomes

Jacob Ames Mar 14, 2016 5:02 PM

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

Actions

Richard Yang @ Jacob Ames on Mar 14, 2016 5:12 PM

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.

Actions

Jeremiah Feist Mar 14, 2016 5:09 PM

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.

Actions

Richard Yang @ Jeremiah Feist on Mar 14, 2016 5:11 PM

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).

Actions

Jeremiah Feist @ Richard Yang on Mar 14, 2016 5:42 PM

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.

Actions

Richard Yang @ Jeremiah Feist on Mar 15, 2016 7:15 AM

Would this allow me to select a section of a part to include in a display state?

Actions

Fred Zobel @ Richard Yang on Mar 15, 2016 4:54 PM

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.

Actions

Jeremiah Feist @ Richard Yang on Mar 15, 2016 10:07 AM

no it will not.

Actions

Greg Hynd Mar 15, 2016 10:13 AM

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.

Actions

Richard Yang Mar 15, 2016 1:50 PM

Actions

Greg Hynd @ Richard Yang on Mar 15, 2016 4:40 PM

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.

Actions

Greg Hynd @ Greg Hynd on Mar 16, 2016 3:56 AM

See picture. hopefully this helps.

Actions

12 Replies

Jacob Ames Mar 14, 2016 5:02 PM
Mark Correct
Correct Answer
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
Like • Show 0 Likes0
Actions
- Richard Yang @ Jacob Ames on Mar 14, 2016 5:12 PM
  Mark Correct
  Correct Answer
  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.
  Like • Show 0 Likes0
  Actions
Jeremiah Feist Mar 14, 2016 5:09 PM
Mark Correct
Correct Answer
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.
Like • Show 0 Likes0
Actions
- Richard Yang @ Jeremiah Feist on Mar 14, 2016 5:11 PM
  Mark Correct
  Correct Answer
  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).
  Like • Show 0 Likes0
  Actions
  - Jeremiah Feist @ Richard Yang on Mar 14, 2016 5:42 PM
    Mark Correct
    Correct Answer
    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.
    Like • Show 0 Likes0
    Actions
    - Richard Yang @ Jeremiah Feist on Mar 15, 2016 7:15 AM
      Mark Correct
      Correct Answer
      Would this allow me to select a section of a part to include in a display state?
      Like • Show 0 Likes0
      Actions
      - Fred Zobel @ Richard Yang on Mar 15, 2016 4:54 PM
        Mark Correct
        Correct Answer
        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.
        Like • Show 0 Likes0
        Actions
      - Jeremiah Feist @ Richard Yang on Mar 15, 2016 10:07 AM
        Mark Correct
        Correct Answer
        no it will not.
        Like • Show 0 Likes0
        Actions
Greg Hynd Mar 15, 2016 10:13 AM
Mark Correct
Correct Answer
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.
Like • Show 0 Likes0
Actions
Richard Yang Mar 15, 2016 1:50 PM
Unmark Correct
Correct Answer
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.
Like • Show 0 Likes0
Actions
- Greg Hynd @ Richard Yang on Mar 15, 2016 4:40 PM
  Mark Correct
  Correct Answer
  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.
  Like • Show 0 Likes0
  Actions
  - Greg Hynd @ Greg Hynd on Mar 16, 2016 3:56 AM
    Mark Correct
    Correct Answer
    See picture. hopefully this helps.
    Like • Show 0 Likes0
    Actions

Using section view made in assembly in a drawing?

Outcomes

Related Content

Recommended Content