What are your most impressive tricks of Solidworks

[matt]

Here's an old school trick:

- In Tools, Options, General, use Single Command Per Pick
- open a sketch
- draw a line, and it turns off the line command after a single line
- double click the line tool on the toolbar, and now you can draw a chain of lines.

Useless? maybe.

[berg_lauritz]

Here's an old school trick:

- In Tools, Options, General, use Single Command Per Pick
- open a sketch
- draw a line, and it turns off the line command after a single line
- double click the line tool on the toolbar, and now you can draw a chain of lines.

Useless? maybe.

You can also double click to not make a sketch line.

[Lucas]

Making a 3Dsketch from bodies:

Create the solid, put the view in Wireframe mode, Box Selection all the edges (or Ctrl+A).
Open 3Dsketch (with everything already selected) and convert entities, then Delete Body.

Is the fastest way to create 3dsketches that I know, and feels kind of hidden because you cant select the edges easily if not in that order.

[Glenn Schroeder]

Making a 3Dsketch from bodies:

Create the solid, put the view in Wireframe mode, Box Selection all the edges (or Ctrl+A).
Open 3Dsketch (with everything already selected) and convert entities, then Delete Body.

Is the fastest way to create 3dsketches that I know, and feels kind of hidden because you cant select the edges easily if not in that order.

Yup. I learned that from @Alin at SW World a few years ago.

[David Matula]

@David Matula, you do know about the Promote function, don't you?

If you have a common subassembly for parts (i.e. you ALWAYS put the together some fasteners with a specific bracket/purchased part), but you don't want to show it on a BOM, you can promote this assembly and it will always dissolve on your BOM and in the drawing.

This also works with virtual assemblies.

Screenshot 2021-08-04 113900.png
Screenshot 2021-08-04 114100.png

It would be best that I do not get to fancy here. Some of the other guys could get really confused. Also not to sure how that would work with Windchill bom, so best to stick with what they know works. Only have a few months left of this contract. So if anyone is looking to hire....

[DanPihlaja]

Not a super trick. Just something that some people might not know about, because I just taught it to about 4 people here.

In fact, it really isn't a Solidworks thing at all, but a Windows thing.

When you are running a program with tabs, like Outlook, Word, Excel, Solidworks.

And specifically, when I say tabs, I mean these:
From Outlook:

From Solidworks:

From Word:

Navigating between tabs can be done in multiple ways:

1) Click on the tab that you want......easy peasy...how everyone does it

2) Put your mouse in the area (with the window active) and roll your mouse wheel. Each roll "click" of the mouse wheel moves one tab over, either right or left.

3) CTRL + Page Up or CTRL + Page Down. Page Down cycles to the right, while Page Up cycles to the left. (works in Solidworks, and most browsers that use tabs (Chrome, Firefox, Edge, etc...), but NOT Outlook, Word, Excel, etc...)

4) Tap the ALT key, then tap one of the corresponding keys to switch to the tab that you want:
Example: To switch to the Layout Tab in Word, tap the ALT key, then tap P

Works in Microsoft stuff, but not in Browsers or Solidworks.

5) In a browser, CTRL + TAB will switch between tabs (because these are actually different pages...so its like switching between different documents in Word, etc...)

[JuTu]

5) In a browser, CTRL + TAB will switch between tabs (because these are actually different pages...so its like switching between different documents in Word, etc...)

OH!? This works in Office products too!? That's new to me.
And in Firefox, Edge and Chrome browsers you can switch between open tabs. Like switching thru open windows in Solidworks.

EDIT: Somehow I feel like I didn't properly read what Dan had written. oh my... oh me...
EDIT2: But then I realised to check and confirm. I works CTRL + TAB changes between windows/tabs in browsers, Office and SW. I learned atleast one new thing today

[Tom G]

(Why to avoid Angle Mates: they flip orientation by themselves, so that they require attention so that your "stable fully defined" assembly remains as you intended it.)

How to avoid Angle Mates

I've figured this one out lately and it's proven itself stable so far. If and only if you desire a 45 degree angle, mate a primary plane as Symmetric between two perpendicular primary planes of an adjacent component. The order of selection matters, so that the first selected entity will be the middle item, and the other two are its "ends". This mate is able to be flipped (intentionally). The major advantage of this method over the method below is that it persists through reorientation of both of the mated components.

(My old method which has minor issues:) Define a reference plane at the desired angle in the assembly, and mate a primary reference plane Parallel to it. This is stable and does not flip by itself, and also can be flipped intentionally. However, if the component is desired to reorient in the assembly, then either the plane needs redefined, or a new reference parallel plane needs created.

Also, you can create a new reference plane in the component (instead of in the assembly) which holds the desired angle, and is then chosen to mate Parallel to other entities.

Furthermore, I strongly avoid Perpendicular, primarily because it cannot flip. Parallel is equally stable and yet more flexible.

[zwei]

So this is something that i stumble by accident today...

You can actually pull the property manager "Out" from the standard tree and put it side by side to the feature tree..
It take up the some display space but i no longer need to have extra click to expand the feature tree to search for the plane or surface that i need...

Now.. if only i can find a way to pin the property manager so that it is always shown even if empty..

[berg_lauritz]

So this is something that i stumble by accident today...

You can actually pull the property manager "Out" from the standard tree and put it side by side to the feature tree..
It take up the some display space but i no longer need to have extra click to expand the feature tree to search for the plane or surface that i need...
image.png

Now.. if only i can find a way to pin the property manager so that it is always shown even if empty..

What the.......

MAGIC! You're too dangerous to be left alive!

[DanPihlaja]

So this is something that i stumble by accident today...

You can actually pull the property manager "Out" from the standard tree and put it side by side to the feature tree..
It take up the some display space but i no longer need to have extra click to expand the feature tree to search for the plane or surface that i need...
image.png

Now.. if only i can find a way to pin the property manager so that it is always shown even if empty..

There are some drawbacks to this. I honestly cannot recall what they were, but they were big enough that I ended up not using it anymore.

If I can remember them, I will post them here.

[bnemec]

There are some drawbacks to this. I honestly cannot recall what they were, but they were big enough that I ended up not using it anymore.

If I can remember them, I will post them here.

When the property manager is docked it grows in width all day, not enough that I notice it right away but when it replaces half the width of the view port I wonder when did that happen?
I sure do wish the feature manager (tree) could be docked and never move or collapse automatically, it seems that I need access to it whenever SW decides to pop it out over the viewport and collapse it. Mostly because there are many things that are easier to select in the feature manager than in the graphics area; or maybe I'm just doing it wrong.

[mike miller]

There are some drawbacks to this. I honestly cannot recall what they were, but they were big enough that I ended up not using it anymore.

If I can remember them, I will post them here.

In my experience, the main drawback is the fact that no matter where you place it, it's either covering up something in the graphics window OR it's too far away. This drawback is greater than the pain of expanding the flyout tree IMHO.

[bnemec]

In my experience, the main drawback is the fact that no matter where you place it, it's either covering up something in the graphics window OR it's too far away. This drawback is greater than the pain of expanding the flyout tree IMHO.

IIRC there's a macro that automatically expands the feature tree each time. But I cannot find it.

[zwei]

In my experience, the main drawback is the fact that no matter where you place it, it's either covering up something in the graphics window OR it's too far away. This drawback is greater than the pain of expanding the flyout tree IMHO.

Interestingly, it had never notice any noticable cover up since i start using this... Maybe because i had been positioning my part center or slightly off-to right by habit (i only realize it when i think about it now...)

The main drawback for me will be the height of the window that is inconsistent which annoy me a little bit

[Lucas]

IIRC there's a macro that automatically expands the feature tree each time. But I cannot find it.

But you will need to run the macro every time to expand it, no? If you find it, please post here. I just got useless Google results... :/

I remember to find this PropertyManager split window when I was looking how to set the Flyout FeatureManager to be the main tree (like others CAD), but unfortunately it's not possible. There's the C shortcut for the Flyout Tree, but it needs to activated first and is kind of useless.

[berg_lauritz]

There are some drawbacks to this. I honestly cannot recall what they were, but they were big enough that I ended up not using it anymore.

If I can remember them, I will post them here.

Tried it out the whole day.

Drawbacks:

• renaming items in the feature tree with F2 is more painful. If you click on the item you have to be FAST to hit F2 otherwise you have to deselect the item & re-select again & quickly hit the button. This seemed to be especially painful in drawings for me.
• The sizing of this seems to be (as are so many things) document specific. And the standard size is tiny so you have to re-size it.

On the positive side:
It is SO MUCH MORE comfortable to work with the feature tree on the left side.... Currently I am happily accepting the drawbacks for this.

[zwei]

Tried it out the whole day.

Drawbacks:

• renaming items in the feature tree with F2 is more painful. If you click on the item you have to be FAST to hit F2 otherwise you have to deselect the item & re-select again & quickly hit the button. This seemed to be especially painful in drawings for me.
• The sizing of this seems to be (as are so many things) document specific. And the standard size is tiny so you have to re-size it.

On the positive side:
It is SO MUCH MORE comfortable to work with the feature tree on the left side.... Currently I am happily accepting the drawbacks for this.

Dint really notice the renaming issue until you mentioned it , it seem to be only specific to drawing view? I have no issue renaming in Part and ASM

FYI, you can actually click on your drawing view → wait for the property manager to pop out → click again and it will allow you to rename (similar to pressing F2)

[Lapuo]

I also remember using this , and then i stopped for some reason which annoyed me , but i cant remember what it was.
I am annoyed because i cant remember it
I used it today , and i works well , so i guess i will continue.

[zwei]

Not sure had it been mention before...

But something that i realize i cant live without recently is binding the Hide All Types (Plane, Sketches, axis, etc) to a keyboard shortcut

Now i just need a macro to hide and show all surfaces body...

[RMcHugh]

Found an error in the macro I posted. Working on it.
I found that the previous code would inadvertently hide a solid body.

The rest of the untested lines have now been commented out and it works as intended for me.
Uncomment a set of these lines to test behavior for a specific surface type.

Ray

[Glenn Schroeder]

If you're going to be using linear patterns in an Assembly, keep in mind the default direction for the pattern. For example, quite a few of my Assemblies are concrete (with rebar) or guardrails. I always place my first rebar, posts, rails, etc on the left side, so when I use a linear pattern I don't need to switch directions. It's a little thing, but can add up if you have multiple patterns, and it's generally just as easy to start on the left as the right.

[Tom G]

This hardly counts as a most impressive trick. All the same, I did not make a new thread for this, and could not find a thread like, "What did you learn that you never knew before?"

Today I learned more lazy.
When entering today's date into custom properties, I typed in the month and date and left out the year by mistake. The date field auto-filled the current calendar year. This is a tiny time saver which is multiplied by the many implemented uses today.

[zwei]

This hardly counts as a most impressive trick. All the same, I did not make a new thread for this, and could not find a thread like, "What did you learn that you never knew before?"

Today I learned more lazy.
When entering today's date into custom properties, I typed in the month and date and left out the year by mistake. The date field auto-filled the current calendar year. This is a tiny time saver which is multiplied by the many implemented uses today.

If you feel a bit "more lazy"
You could setup a autohotkey to key in today date in the format you need

I originally setup mine to key in date in DD-MMM-YYYY format in all caps and had ever bother about checking the date when filling my rev table

[the_h4mmer]

(Why to avoid Angle Mates: they flip orientation by themselves, so that they require attention so that your "stable fully defined" assembly remains as you intended it.)

How to avoid Angle Mates

I've figured this one out lately and it's proven itself stable so far. If and only if you desire a 45 degree angle, mate a primary plane as Symmetric between two perpendicular primary planes of an adjacent component. The order of selection matters, so that the first selected entity will be the middle item, and the other two are its "ends". This mate is able to be flipped (intentionally). The major advantage of this method over the method below is that it persists through reorientation of both of the mated components.

Furthermore, I strongly avoid Perpendicular, primarily because it cannot flip. Parallel is equally stable and yet more flexible.

What about using the mid-plane relation between your perpendicular primary planes for a reference plane and then adding a coincident mate? I guess it would add another feature, but wonder if it would be more advantageous or if there are hidden drawbacks. I don't know that I'll have any use case to test either method out soon, but just curious if anyone would know offhand.

[the_h4mmer]

Maybe this is a silly "trick" to mention, but I think I use the space bar more than any shortcut for reorienting the model view. I use it so much that the SpaceMouse I have has become pretty obsolete (I might use it if it had more hotkeys I could configure).

I'm also a fan of:
- Design Checker tool (especially great for drawing consistency)
- Symmetry Check tool
- Creating a Config for 'simplified' geometry (suppress any features not needed/visible)
- Embossing 3D printed parts with PDM file version to track the physical versions
- Design History (especially looking at feature properties to see who made the last changes and/or when)
- Zebra stripes
- Surfacing tools (they can be a headache but also be a tremendous help)

Best of all, I love the "Please wait, Solidworks is busy" message, since it's my reminder that I should stop every so often to stretch or go get some water.

[Tom G]

What about using the mid-plane relation between your perpendicular primary planes for a reference plane and then adding a coincident mate? I guess it would add another feature, but wonder if it would be more advantageous or if there are hidden drawbacks.

I've done that before, both in assembly reference planes and in component reference planes. It is also very stable, and also available in lightweight mode because it is a reference entity. I prefer parallel to coincident for axial orientation.
Early on as a novice, I received a series of van stone flange parts which had their hole pattern in a diamond (+) instead of a square (x). I already began using this in projects, then later added mid-plane 45º planes to use as substitute-top and substitute-right planes. It remains this way, and mates stably even if this is an outlier in the library as not compliant with import standards developed later.

[blanke]

When the property manager is docked it grows in width all day, not enough that I notice it right away but when it replaces half the width of the view port I wonder when did that happen?
I sure do wish the feature manager (tree) could be docked and never move or collapse automatically, it seems that I need access to it whenever SW decides to pop it out over the viewport and collapse it. Mostly because there are many things that are easier to select in the feature manager than in the graphics area; or maybe I'm just doing it wrong.

Maybe a bit late, but I encountered the same problem as you described. I've found a macro which could change the width of the feature manager design tree. The only downside was that if you have placed the property manager side by side with the feature manager, it would only change the feature manager width. So I started looking into docking the property manager with VBA and adjusted the code so that the property manager first docks to the original location and then change the width. This will change the width of both the property and feature manager. After this step it wil dock the windows side by side again. Lastly it will change the width of the feature manager design tree once more. Because the windows are side by side, the width of the property manager will not change. There is a standard width in this code of 350 pixels for both windows which can be adjusted to your preference independently.

Macro code:

Code: Select all

'----------------------------------------
'
' Preconditions:		Model document is open.
'
' Postconditions:	Width of featuremanager design  tree and property manager are controlled by WidthFeat and WidthProp (default 350)
'				Property manager is docked side by side with the featuremanager (position 2)
'
'
' Notes:            When you work with the property manager side by side with the feature manager design tree
'                   sometimes the width of this window will grow over time. You can adjust the width of the feature
'                   manager design tree, but this will not chanage the width of the property manager when docked side by side.
'                   This macro first docks the property manager on the original position, then changes width and docks it side by side.
'                   After docking it will change the width of the feature manager once more, if you would like a different width of this.
'
'                   If you want to change the docking location you can chanage the number at the end of the last line.
'                   0 = original, 1 = bottom left, 2 = side by side
'
'----------------------------------------
Option Explicit

Sub main()

    Dim swApp                   As SldWorks.SldWorks
    Dim swModel                 As SldWorks.ModelDoc2
    Dim nWidth                  As Long
    Dim nRetVal                 As Long
    Dim WidthProp               As Integer
    Dim WidthFeat               As Integer
    Dim Part                    As Object
    
    Set swApp = CreateObject("SldWorks.Application")
    Set swModel = swApp.ActiveDoc
    
    Set Part = swApp.ActiveDoc
    Dim myModelView As Object
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    
    'Property manager is docked on original location, same place as feature manager design tree
    swApp.SetUserPreferenceIntegerValue swUserPreferenceIntegerValue_e.swPropertyMgrDockingState, 0
    
    'Reading old width
    nWidth = swModel.GetFeatureManagerWidth
    
    'Writing width of property manager
    WidthProp = 350
    nRetVal = swModel.SetFeatureManagerWidth(nWidth / nWidth * WidthProp)

    'docking property manager side by side with feature manager design tree (Position 2)
    swApp.SetUserPreferenceIntegerValue swUserPreferenceIntegerValue_e.swPropertyMgrDockingState, 2
    
    'Writing width of feature manager
    WidthFeat = 350
    nRetVal = swModel.SetFeatureManagerWidth(nWidth / nWidth * WidthFeat)
    
End Sub

[bnemec]

Maybe a bit late, but I encountered the same problem as you described. I've found a macro which could change the width of the feature manager design tree. The only downside was that if you have placed the property manager side by side with the feature manager, it would only change the feature manager width. So I started looking into docking the property manager with VBA and adjusted the code so that the property manager first docks to the original location, then change the width and docks it side by side again. Lastly it will change the width of the feature manager design tree once more. Because the windows are side by side, the width of the property manager will not change. There is a standard width in this code of 350 pixels for both windows which can be adjusted to your preference independently.

Macro code:

Code: Select all

'----------------------------------------
'
' Preconditions:    Model document is open.
'
' Postconditions:   Width of featuremanager design  tree and property manager is controlled by myWidth (default 350)
'                   Property manager is docked side by side with the featuremanager (position 2)
'
'
' Notes:            When you work with the property manager side by side with the feature manager design tree
'                   sometimes the width of this window will grow over time. You can adjust the width of the feature
'                   manager design tree, but this will not chanage the width of the property manager when docked side by side.
'                   This macro first docks the property manager on the original position, then changes width and docks it side by side.
'                   After docking it will change the width of the feature manager once more, if you would like a different width of this.
'
'                   If you want to change the docking location you can chanage the number at the end of the last line.
'                   0 = original, 1 = bottom left, 2 = side by side
'
'----------------------------------------
Option Explicit

Sub main()

    Dim swApp                   As SldWorks.SldWorks
    Dim swModel                 As SldWorks.ModelDoc2
    Dim nWidth                  As Long
    Dim nRetVal                 As Long
    Dim WidthProp               As Integer
    Dim WidthFeat               As Integer
    Dim Part                    As Object
    
    Set swApp = CreateObject("SldWorks.Application")
    Set swModel = swApp.ActiveDoc
    
    Set Part = swApp.ActiveDoc
    Dim myModelView As Object
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    
    'Property manager is docked on original location, same place as feature manager design tree
    swApp.SetUserPreferenceIntegerValue swUserPreferenceIntegerValue_e.swPropertyMgrDockingState, 0
    
    'Reading old width
    nWidth = swModel.GetFeatureManagerWidth
    
    'Writing width of property manager
    WidthProp = 350
    nRetVal = swModel.SetFeatureManagerWidth(nWidth / nWidth * WidthProp)

    'docking property manager side by side with feature manager design tree (Position 2)
    swApp.SetUserPreferenceIntegerValue swUserPreferenceIntegerValue_e.swPropertyMgrDockingState, 2
    
    'Writing width of feature manager
    WidthFeat = 350
    nRetVal = swModel.SetFeatureManagerWidth(nWidth / nWidth * WidthFeat)
    
End Sub

Because I find none of the docked property manager options favorable, I have it undocked and out to the left of the parent solidworks window. It's a long way over to it but it is the only option that doesn't hide the feature/assembly tree AND is consistent. I can get used to nuisance behavior if it's consistent but random nuisance behavior can be frustrating and counter productive.

[bnemec]

This thread title always makes me think of this meme. It's about where I'm at with SW:

[azreal1031]

Over the past few months I find myself coming back to this thread over and over again. There's just too much knowledge here to pass up! On a related note, you can double click a face in a part or an assembly, and it'll show all the driving dimensions. I don't know how fast you are with the measure tool, but this has came in handy quite a few times for a quick reference.

On another note, double clicking a feature just selects the whole part.

[Tera]

you can double click a face in a part or an assembly, and it'll show all the driving dimensions.

For me it shows all Driving and Driven dimensions.

[Jaylin Hochstetler]

Over the past few months I find myself coming back to this thread over and over again. There's just too much knowledge here to pass up! On a related note, you can double click a face in a part or an assembly, and it'll show all the driving dimensions. I don't know how fast you are with the measure tool, but this has came in handy quite a few times for a quick reference.

On another note, double clicking a feature just selects the whole part.

FYI, if you click on one of the dimension you can change it.

[azreal1031]

FYI, if you click on one of the dimension you can change it.

It just keeps getting better.

[MadMike]

Here's a GIF of a really fast way to add intersection relations!Intersection.gif

Can't see the GIF now, can you re-upload or describe?

[JSculley]

It just keeps getting better.

If you turn on Instant3D you only have to click a face once. And you can drag the blue 'handles' to alter the dimensions. See Instant2D as well.

[zxys001]

Every time I've used it I get a mixed reaction and I tend to turn it off because it's not always clear, and I feel like I spend too much time trying to dissect using it or I rarely need it.
BUT, it's a good thing to have for clues if you are trying to preserve or workaround a parent/child issue.

https://help.solidworks.com/2021/englis ... TE_NEW.htm

[Glenn Schroeder]

FYI, if you click on one of the dimension you can change it.

. . . or if you left click on it you can select "Configure dimension" from the drop-down to bring up a simplified design table, which can be very helpful if you work with configurations.

[berg_lauritz]

Just stumbled upon this again when trying out some tricks @Dwight showed us here and I'm glad I remembered:

Right clicking a sketch pattern gives you the option to edit it:

2022-06-03 09_55_42-.png (14.56 KiB) Viewed 12718 times

Edit:
As the master himself pointed out:

I sometimes get tripped up by right-clicking the relation, which doesn't work. To be clear, you have to right-click a sketch element in the pattern, not the pattern relation icon.

Dwight

[Dwight]

Right clicking a sketch pattern gives you the option to edit it:

I sometimes get tripped up by right-clicking the relation, which doesn't work. To be clear, you have to right-click a sketch element in the pattern, not the pattern relation icon.

Dwight

[Glenn Schroeder]

I found a trick a while ago that I've used a few times. I know we can only break extension leaders around other dimensions, but I figured out a way to get it done if I need to break them around other leaders (notes, weld symbols, etc). I place the other annotation, then add a dimension that I really don't need, with it's extension line crossing the extension line of the one I want to break, at the location I want it to break.

Set the original dimension to break extension lines, then hide the new one. The break will stay there, even with the dimension it's breaking around hidden.

If someone unfamiliar with this opens the drawing later they might have a lot of fun figuring out what's going on. That's just a bonus.

[DennisD]

I found a trick a while ago that I've used a few times. . .

If someone unfamiliar with this opens the drawing later they might have a lot of fun figuring out what's going on. That's just a bonus.

Perfect!

[JSculley]

I found a trick a while ago that I've used a few times. I know we can only break extension leaders around other dimensions, but I figured out a way to get it done if I need to break them around other leaders (notes, weld symbols, etc). I place the other annotation, then add a dimension that I really don't need, with it's extension line crossing the extension line of the one I want to break, at the location I want it to break.

I would argue that there is always a solution that doesn't require this, requires less work and doesn't evoke hatred in future generations.

Also, I hate your drawings. Nothing personal. They just rub me the wrong way. Mixed case and periods at the end of annotations? I need eye bleach.

[Glenn Schroeder]

I would argue that there is always a solution that doesn't require this, requires less work and doesn't evoke hatred in future generations.

Also, I hate your drawings. Nothing personal. They just rub me the wrong way. Mixed case and periods at the end of annotations? I need eye bleach.

That's fair. I don't always use periods, unless the note is a complete sentence.

And I hate all caps. It always looks like shouting. I know it's widely regarded as the best practice, but I still don't like it, and in 13 years I haven't received any complaints about it from clients or suppliers.

By the way, I dimension to hidden lines also. I'd like to see how the people who made that rule would show rebar placement in concrete.

[berg_lauritz]

[...] And I hate all caps. It always looks like shouting. [...]

I agree. I am constantly shouting in my head at work because we use all caps. And it's annoying if you write somebody a text message with all caps on. It's like forgetting to take the ear plugs out and SHOUT!

[JSculley]

That's fair. I don't always use periods, unless the note is a complete sentence.
in 13 years I haven't received any complaints about it from clients or suppliers.

I'm just writing what they are all thinking.

By the way, I dimension to hidden lines also. I'd like to see how the people who made that rule would show rebar placement in concrete.

Section views. Or by flipping the script and showing the rebar as solid and the surrounding concrete as phantom/hidden.

But these are large projects where they are probably using a dedicated tool for that kind of thing. SW doesn't do well with lots of detail and section views, so your approach is probably for the best.

[colt]

Doing assembly cut "up to surface".

This one is hidden unless you know the trick for parts: double clicking on a surface will select the end condition of "up to surface". I don't think this is technically supported because there is no formal item in end condition dropdown menu. Double click on the surface you want to cut up to while editing an assembly cut extrude. Just like it works for parts, it will convert the assembly extrude cut to "up to surface". The end condition dropdown menu will be blank but the feature will still succeed. (if you close and reopen the feature then "up to surface" is available in the dropdown)

[Glenn Schroeder]

Not mine, but @Alin's.

[Frederick_Law]

And I hate all caps. It always looks like shouting.
By the way, I dimension to hidden lines also. I'd like to see how the people who made that rule would show rebar placement in concrete.

Yes, my drawings don't scream. No ALL CAPS !!!!!

Hidden line dimension. Only when necessary.
Of course, use a view with more visible lines.

[Alin]

Not mine, but @Alin's.

Not mine, but @matt 's . It is in the Bible.