How to create section views

[KSHansen]

I've been watching videos for about an hour and a half, and they all seem to be some variation of "draw your cutting plane line on a view, then drop your new view somewhere." But I have other questions...

A new section view has to be projected from your cutting plane. Is there any way to break that association? I don't have room for a new view in that direction.

Does my section have to be projected from an existing view? Can't I just add a view where the part is rotated 15 degrees from vertical, and section it? No?

How do I show just a small portion of my section view? I only need this view so I can add two dimensions that are one little corner of the part.

[Glenn Schroeder]

1. If you mean to break the alignment with the parent view, then yes. Right-click on the Section View and you'll see an option in the drop-down (see below). After selecting that you can move the view around however you want.

In the future, when first creating a section view if you hold down Ctrl before clicking to place it that will disable the default alignment and you can place the view where you want right away.

2. As far as I know you need a parent view to create a section view. However, if you really want to you can insert a drawing view, create a section view from it, then Hide the parent view.

3. You can crop a section view and increase the scale, or create a Detail View from the Section View, depending on what works best for your situation.

[mike miller]

You can also do a Broken-out Section view if you want only a small area sectioned. This is defined by a contour and a cut depth.

[Tom G]

2. As far as I know you need a parent view to create a section view. However, if you really want to you can insert a drawing view, create a section view from it, then Hide the parent view.

Nice answer Glenn. I would add that the parent view also needs to be on the same sheet as its derived Section view. I often have these outside of the sheet border, and hidden. Large plan takes up whole 1st sheet. The same plan view is pasted into other sheets as a parent to create sections from.

The CTRL placement tip to break default alignment is a new one to me, and will be very helpful. Before, I had reoriented (rotated) the hidden parent plan views to end up with the section aligned where I want it on the sheet.

[Dwight]

You can also create a section view in the model then show it in the drawing.

[Glenn Schroeder]

Nice answer Glenn. I would add that the parent view also needs to be on the same sheet as its derived Section view. I often have these outside of the sheet border, and hidden. Large plan takes up whole 1st sheet. The same plan view is pasted into other sheets as a parent to create sections from. . . .

I'm afraid you're mistaken about that. You don't need to go to all that trouble of copying the parent view and pasting it on another sheet.

After placing a Section View on the sheet with the parent view you can click on it in the tree, drag to another sheet name, and drop. That will move the section view to the other sheet, leaving the parent view on the original sheet, and it will still be parametric. The sheet with the section view and parent view has to be active while doing this.

I do that all the time with section views showing concrete and rebar.

[Tom G]

Well gobsmack me. Thank you again. This thread has helped a lot.

[Glenn Schroeder]

Well gobsmack me. Thank you again. This thread has helped a lot.

I'm glad I could help. By the way, that method of moving views from one sheet to another works for all kinds of views (as far as I know), not just section views.

[KSHansen]

1. If you mean to break the alignment with the parent view, then yes. Right-click on the Section View and you'll see an option in the drop-down (see below). After selecting that you can move the view around however you want.

In the future, when first creating a section view if you hold down Ctrl before clicking to place it that will disable the default alignment and you can place the view where you want right away.

2. As far as I know you need a parent view to create a section view. However, if you really want to you can insert a drawing view, create a section view from it, then Hide the parent view.

3. You can crop a section view and increase the scale, or create a Detail View from the Section View, depending on what works best for your situation.

1. Excellent. I should have been able to find that one on my own.
2. Good to know
3. Crop view is what I was looking for. Strange that you have to select your sketch before hitting the Crop View button, and not the view itself.

I can't change the length of my cutting plane line? You know, move the arrows up or down? Or break extension lines where I want?

Thanks to everyone for all the help! Next question, is there any way to rotate a view? You know, make it upright, instead of at the angle that the auxiliary view plane places it?

[jcapriotti]

No parent view required:

[SPerman]

I can't change the length of my cutting plane line? You know, move the arrows up or down? Or break extension lines where I want?

See if this helps.

[Glenn Schroeder]

1. Excellent. I should have been able to find that one on my own.
2. Good to know
3. Crop view is what I was looking for. Strange that you have to select your sketch before hitting the Crop View button, and not the view itself. I can understand it. What if you have extra sketch elements in the view?

I can't change the length of my cutting plane line? You know, move the arrows up or down? Or break extension lines where I want? Right-click on the section line and select "Edit Crop" from the drop-down. Rebuild when finished.

Thanks to everyone for all the help! Next question, is there any way to rotate a view? You know, make it upright, instead of at the angle that the auxiliary view plane places it? Click on the view to select it, then click on the icon shown below in the heads-up toolbar (my user interface is heavily customized, but I think that one is there out-of-the-box. If not you should be able to do a search for "Rotate"). That will open up a small dialog box that will allow you to enter the value of the desired rotation angle. It will rotate counter-clockwise, so enter the value accordingly. It will accept negative values.

[DanPihlaja]

... would add that the parent view also needs to be on the same sheet as its derived Section view....

No, it actually doesn't. You can have a section view on a different sheet than the originating view.

See the attached GIF file (Click on it below to view it).

Edit: And I see that Glenn beat me to it. LOL

[KevinC]

See if this helps.

Additionally, you can right click the line and select Edit cutting line then Edit sketch.
This will also allow you to see any relations and add/remove them, too.

[KevinC]

is there any way to rotate a view? You know, make it upright, instead of at the angle that the auxiliary view plane places it?

In addition to Mr. Schroeder's reply (and, yes, Rotate View in the HUD is OOTB), you can also right click a view and select:

This dialog appears (same as in Mr. Schroeder's post):

image.png (7.66 KiB) Viewed 4500 times

The angle is absolute, not incremental.
For example, you need to rotate 90° so you enter 90 and click Apply, but it's the wrong 90°.
Two more clicks on Apply won't get you there. Once at the specified angle, subsequent clicks to Apply do nothing.
In this case, you'd enter 270 and then click Apply.

[KevinC]

Also, when you move child views to a different sheet, be sure to add a location label. You can also use them on the same sheet if needed.
These are dynamic and will update with the current position and sheet.

Click each parent and child. For a crop, you must click the profile.

After I drag the child view, in the tree, from sheet 1 to sheet 2.
The sheet number updates (I didn't relocate either view, the zones remained the same):

[Glenn Schroeder]

. . . The angle is absolute, not incremental.
For example, you need to rotate 90° so you enter 90 and click Apply, but it's the wrong 90°.
Two more clicks on Apply won't get you there. Once at the specified angle, subsequent clicks to Apply do nothing.
In this case, you'd enter 270 and then click Apply.

. . . or enter -90. That will do the same thing (I mentioned above that you can enter negative values).

[KevinC]

You can also do a Broken-out Section view if you want only a small area sectioned. This is defined by a contour and a cut depth.

2021-12-03 14_04_22.jpg

This answers the last question in your OP.

[KevinC]

. . . or enter -90. That will do the same thing (I mentioned above that you can enter negative values).

Thank you, I missed that, but I do recall having done that.

[Tom G]

You can also create a section view in the model then show it in the drawing.

No, I cannot @Dwight , using SWx 2018 SP5. Is this newer?
I preferred this method among others on this page because the assembly environment is far faster and responsive than the slow drawing environment.
I assumed this would work as suggested. And made a handful of saved views (XX SevtionView1, XX SectionView2, etc) in my assembly before testing this out.

I created four section views in the assembly, saved them as views, inserted those views into the drawing, and it is not showing as section cut, but rather merely showing an outside elevation from that same direction. The saved views are reproduced accurately only in the assembly environment.

Please elaborate. What version are you using to accomplish this? Your suggested workflow appeared direct and simple enough, so am I misunderstanding what you mean by "create a section view in the model"? Are you only talking about parts, or assemblies also? It is not working.

[SPerman]

Same for me in 2020 SP5. I don't see anything in the help that talks about this workflow either.

[Dwight]

Tom

You are right. I had thought I'd seen that done in a presentation, and I have occasionally used saved section views, but I never did use one in a drawing. I see now that help does say that you can't use them in drawings.

Sorry for the misstatement.

Dwight

[KevinC]

Tom

You are right. I had thought I'd seen that done in a presentation, and I have occasionally used saved section views, but I never did use one in a drawing. I see now that help does say that you can't use them in drawings.

Sorry for the misstatement.

Dwight

I don't know where in Help it states this, but section views saved within a model can be used in a drawing and are dynamic to changes in the model's section view. To do this follow these steps:
At the bottom of the section PM, click Save:

This dialog displays with "Drawing annotation view" not checked:

image.png (6.79 KiB) Viewed 4372 times

Check "Drawing annotation view" and the name automatically changes to the "normal" section naming.
You can change this, but I usually don't. Also, for each save, this name will increment the section letters.
Also, if you don't uncheck the first tickbox then this view will also be saved within the model (available on the Orientation dialog):

image.png (7.2 KiB) Viewed 4372 times

Save your file and in the drawing refresh the views, if needed, and you'll see a cutting line view and a section view for each saved section:

The caveat is that you must place the cutting line view onto the drawing before placing any saved section view.
As you are dragging the cutting line view onto the drawing, the cut lines will be visible, but after you place the view, you won't see any cut lines in the view. This is normal. These will show later.
Also, the cutting line view is no longer in the view palette:

Drag each saved section view from the palette and onto the drawing.
As each of these views is placed, its cutting line will automatically be shown in the parent cutting view:

[Glenn Schroeder]

No, I cannot @Dwight , using SWx 2018 SP5. Is this newer?
I preferred this method among others on this page because the assembly environment is far faster and responsive than the slow drawing environment.
I assumed this would work as suggested. And made a handful of saved views (XX SevtionView1, XX SectionView2, etc) in my assembly before testing this out.

I created four section views in the assembly, saved them as views, inserted those views into the drawing, and it is not showing as section cut, but rather merely showing an outside elevation from that same direction. The saved views are reproduced accurately only in the assembly environment.

Please elaborate. What version are you using to accomplish this? Your suggested workflow appeared direct and simple enough, so am I misunderstanding what you mean by "create a section view in the model"? Are you only talking about parts, or assemblies also? It is not working.

You can always just create a second configuration in the Assembly, make a simple extruded cut that's suppressed in the main configuration, and use this configuration as the section view in the Drawing.

[KevinC]

No, I cannot @Dwight , using SWx 2018 SP5. Is this newer?
I preferred this method among others on this page because the assembly environment is far faster and responsive than the slow drawing environment.
I assumed this would work as suggested. And made a handful of saved views (XX SevtionView1, XX SectionView2, etc) in my assembly before testing this out.

I created four section views in the assembly, saved them as views, inserted those views into the drawing, and it is not showing as section cut, but rather merely showing an outside elevation from that same direction. The saved views are reproduced accurately only in the assembly environment.

Please elaborate. What version are you using to accomplish this? Your suggested workflow appeared direct and simple enough, so am I misunderstanding what you mean by "create a section view in the model"? Are you only talking about parts, or assemblies also? It is not working.

Unless the section views are saved as a "Drawing annotation view" (as I showed in a previous post) then these views will not be available in the drawing view palette.
This method has worked for me for parts and for assemblies.

[Dwight]

Unless the section views are saved as a "Drawing annotation view" (as I showed in a previous post) then these views will not be available in the drawing view palette.
This method has worked for me for parts and for assemblies.

Yes. In help it states that when using "View Orientation" the views cannot be used in a drawing. As you say, using "Drawing annotation view " does work.