What are your most impressive tricks of Solidworks

[Frederick_Law]

What, you mean SW went and did some different than the rest of the pc world and assigned tab and Shift tab to something other than cycling through "tabs", windows or applications on the taskbar?

It is an innovative company. It had to do things differently.
Like not all UI control behave the same way.
Next innovation, new keyboard layout.

[Jaylin Hochstetler]

Press "windows" key + V to view your clipboard. You can also pin items to your clipboard by clicking on the 3 dots on the item in the clipboard and clicking "Pin".

2021-03-24 08_05_50-Window.jpg

I use this all the time when I am copying and pasting multiple items.

[DanPihlaja]

Did you know about the "New Window" functionality? See the attached GIF video.

FYI, this is usable for so much more than just Assembly mating.....

NewWindow.gif

[KevinC]

When using mirror sketch entities, if you preselect the mirroring entity along with the to-be-mirrored bits, the mirror happens without the mirror PM opening (assuming SW can figure out the correct mirror-by entity from the selection).

Oddly, this doesn't work in mirror component (possibly because of the subsequent mirror choices), but if you do preselect all, the mirror PM does open with the mirror-by box filled in and with the to-be-mirrored bits in their list.

Kevin

[KevinC]

Press "windows" key + V to view your clipboard. You can also pin items to your clipboard by clicking on the 3 dots on the item in the clipboard and clicking "Pin".
2021-03-24 08_05_50-Window.jpg
I use this all the time when I am copying and pasting multiple items.

I too run with this on...love it. I use the keyboard to do a Ctrl+C and then go to paste with a Ctrl+V and hit Ctrl+C again with nothing selected and would lose the previous clip.
Another aspect is that you can "collect" several copies at a time and then paste each without having to do multiple copy/switch/paste.

I believe this is off by default though.
To turn on, go to (Windows) Settings>System>Clipboard.

Kevin

[Jaylin Hochstetler]

Press "windows" key + V to view your clipboard. You can also pin items to your clipboard by clicking on the 3 dots on the item in the clipboard and clicking "Pin".
2021-03-24 08_05_50-Window.jpg
I use this all the time when I am copying and pasting multiple items.

I too run with this on...love it. I use the keyboard to do a Ctrl+C and then go to paste with a Ctrl+V and hit Ctrl+C again with nothing selected and would lose the previous clip.
Another aspect is that you can "collect" several copies at a time and then paste each without having to do multiple copy/switch/paste.

I believe this is off by default though.
To turn on, go to (Windows) Settings>System>Clipboard.

Kevin

To speed it up even more I have it as a gesture on my mouse, as you can see earlier in this thread.

[mike miller]

Did you know about the "New Window" functionality? See the attached GIF video.

FYI, this is usable for so much more than just Assembly mating.....

NewWindow.gif

I'm not sure I want to sacrifice real-estate on my 32" curved-screen monitor.........

[Harris]

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

Intersection.gif

[Roasted By John]

1. The use of a Skeleton Sketch part - Eliminates Circular Rebuilds, Better Models, Parametric Changes and a lot of other plus's
2. Multiple Sheet Drawing - If you have a 100 different/unique parts, it's nice to open one file instead of a 100...
3. Custom Property Tab Builder - To track custom properties in parts and assemblies individually
4. Macros - get all the macros you can and use them in your workflow
5. Task Scheduler
6. #Task http://www.centralinnovation.com.au/
7. Mouse Gestures
8. S Key
9. Layers (Colored)
10. Templates
11. Isolate
12. Use Colored Sketches (thanks to Alin Vargatu )
Plus a lot more

[mike miller]

1. The use of a Skeleton Sketch part - Eliminates Circular Rebuilds, Better Models, Parametric Changes and a lot of other plus's
2. Multiple Sheet Drawing - If you have a 100 different/unique parts, it's nice to open one file instead of a 100...
3. Custom Property Tab Builder - To track custom properties in parts and assemblies individually
4. Macros - get all the macros you can and use them in your workflow
5. Task Scheduler
6. #Task http://www.centralinnovation.com.au/
7. Mouse Gestures
8. S Key
9. Layers (Colored)
10. Templates
11. Isolate
12. Use Colored Sketches (thanks to Alin Vargatu )
Plus a lot more

What is #Task? I've heard of it but never seen it.

[Roasted By John]

Macro source

[Jaylin Hochstetler]

I have a Logitech MX Master (I absolutely love it) mouse that I have 10 gestures mapped on it. It greatly speeds things up mostly in other programs as I use the SW mouse gestures setup in SW. I'd really like a 3D mouse but that costs money and I'm guessing y'all know how it goes when engineers need things!

Here's what my Logitech gestures look like:
2021-03-16 12_49_01-Logitech Options.jpg2021-03-16 12_48_40-Logitech Options.jpg
Edit: One thing I use a lot is the button I have assigned as "Enter". This way I can close dialogues with out moving my mouse or hitting the "Enter" key on my keyboard (I never quite understood why they don't put another "Enter" button on the left so you don't have to take your hand off your mouse.) Saves a little bit of time and mouse miles.

I also use SW keyboard shortcuts for the common commands.

Hey, I actually convinced management to get me a 3D Connexion compact mouse. Still tryin' to get the hang of it, but love it so far.

[HerrTick]

Boolean the hard way!

Got a feature that absolutely refuses to unite/subtract/intersect? Turn the solids into surfaces using Delete Face or other means. Trim pieces to match. Then knit into a solid.

The true miracle is that SW will recognize the result as the same solid after the knit operation.

[HerrTick]

Sometimes STEP export turns planes and revolves into B-surfaces. That sucks, but there's a simple, stupid fix:
Export as STEP203 and reimport. Often this re-translates the B-surfaces into revolves and planes. Why? I don't know.

This also works on other CAD platforms. Used this is NX recently.

[Rob]

Annotations not working?

A ref point can step up..

image.png

[mbiasotti]

@HerrTick Got a feature that absolutely refuses to unite/subtract/intersect?

When I run into this problem, what I do is make a surface copy of the opposite face of the Solid that I'm trying to unite (say a mirrored body across the midplane that won't unite). With that surface, I then do a Replace Face on the face of the solid I want to unite with the opposition solid - work 98% of the time.

[Alin]

@HerrTick Got a feature that absolutely refuses to unite/subtract/intersect?

When I run into this problem, what I do is make a surface copy of the opposite face of the Solid that I'm trying to unite (say a mirrored body across the midplane that won't unite). With that surface, I then do a Replace Face on the face of the solid I want to unite with the opposition solid - work 98% of the time.

Wow! Never thought of that, but, now, I can't wait to try it! Thanks @mbiasotti !!!

[HerrTick]

Great add, Mark. Many thanks.

There's also an important topology lesson there. SW and the parasolid kernel hate hate HATE when things ALMOST match. The replace face trick turns an *almost* into an EXACT match.

[JuTu]

My most impressive trick with Solidworks? Youtube

One of the most overwhelming experience was wathing one of those vids named "60 tips in 60 minutes"

[mattpeneguy]

My most impressive trick with Solidworks? Youtube

One of the most overwhelming experience was wathing one of those vids named "60 tips in 60 minutes"

Also, you can learn a bunch of tricks by watching the Model Mania videos. Just search model mania solidworks and it turns up.

[DanPihlaja]

I have a Logitech MX Master (I absolutely love it) mouse that I have 10 gestures mapped on it. It greatly speeds things up mostly in other programs as I use the SW mouse gestures setup in SW. I'd really like a 3D mouse but that costs money and I'm guessing y'all know how it goes when engineers need things!

Here's what my Logitech gestures look like:
2021-03-16 12_49_01-Logitech Options.jpg2021-03-16 12_48_40-Logitech Options.jpg
Edit: One thing I use a lot is the button I have assigned as "Enter". This way I can close dialogues with out moving my mouse or hitting the "Enter" key on my keyboard (I never quite understood why they don't put another "Enter" button on the left so you don't have to take your hand off your mouse.) Saves a little bit of time and mouse miles.

I also use SW keyboard shortcuts for the common commands.

Hey, I actually convinced management to get me a 3D Connexion compact mouse. Still tryin' to get the hang of it, but love it so far.

I am using the big fat one with a wire and everything. I had to buy it myself because they saw that mice were less than $10 for cheap Microsoft ones. So, I now have 2 of them because I won one at SW headquarters 2 years ago.

[AlexLachance]

Here's a really neat trick for all you people working assembly drawings with multiple section views. Doing so should speed up your drawings considerably. *It can only be done if you do not work with surfaces or if you work with them in specific contexts that do not require them in section views*


Turn off surfacic bodies inside your section views. You will see a huge difference in drawing performance.

[Glenn Schroeder]

I don't know if this is exactly a trick, but similar to the way most experienced users will say to not use a 3d sketch unless you really need a 3d sketch, I model on the principle of only using an equation if I really need one.

For one common example, if I'm sketching and want two equal dimensions I don't use an equation. Instead I'll add two construction lines and give them an equal relation to accomplish the same purpose.

Come to think of it, I'm a big believer in using construction lines and relations instead of dimensions in general whenever possible, not just to avoid equations.

[DennisD]

I don't know if this is exactly a trick, but similar to the way most experienced users will say to not use a 3d sketch unless you really need a 3d sketch, I model on the principle of only using an equation if I really need one.

For one common example, if I'm sketching and want two equal dimensions I don't use an equation. Instead I'll add two construction lines and give them an equal relation to accomplish the same purpose.

Come to think of it, I'm a big believer in using construction lines and relations instead of dimensions in general whenever possible, not just to avoid equations.

Along those lines I will often use Link Dimension to set two or more dimensions to be the same. This is especially valuable when you cannot easily achieve this with construction geometry. It is also configurable.

[Rob]

I just discovered that the selection filter 'remembers' your selections in the sketch environment separately.

This mitigates SW frustrating behaviour of prioritising model vertices over visible sketch points.



exit the sketch - the filters clear

[JuTu]

1. The use of a Skeleton Sketch part - Eliminates Circular Rebuilds, Better Models, Parametric Changes and a lot of other plus's
2. Multiple Sheet Drawing - If you have a 100 different/unique parts, it's nice to open one file instead of a 100...
3. Custom Property Tab Builder - To track custom properties in parts and assemblies individually
4. Macros - get all the macros you can and use them in your workflow
5. Task Scheduler
6. #Task http://www.centralinnovation.com.au/
7. Mouse Gestures
8. S Key
9. Layers (Colored)
10. Templates
11. Isolate
12. Use Colored Sketches (thanks to Alin Vargatu )
Plus a lot more

1. Note to self: Learn this!
3. This so awesome! Just couple of days ago I drafted first versions of tabs and yesterday gave them around for trial run. More info at a glance!
4. Still ahead for me.
7. My favorite number is twelve
8. How many more commands I still could include?

While working with assemblies Component Preview window is great to align parts for mating.

Also, customizing View aka HUD. I've put all those, that I don't need all the time but still use, features and other drop-down/flyout capable tools closer.

[Glenn Schroeder]

I just posted something on another thread that reminded me of a couple shortcuts I found years ago that others may not be aware of.

When I want to create an Extruded Boss/Base or Extruded Cut my usual workflow is to select the face or plane first, then the feature. That opens a sketch on the selected plane or face, and then the property manager for the feature opens automatically when I close the sketch.

I do something similar when using the Hole Wizard. I select the face first, then the feature. When I go to the second page of the property manager the sketch point tool is automatically active. I don't know that this one really saves any clicks, but it certainly eliminates the possibility of making it a 3d sketch by mistake.

[JuTu]

When I want to create an Extruded Boss/Base or Extruded Cut my usual workflow is to select the face or plane first, then the feature. That opens a sketch on the selected plane or face, and then the property manager for the feature opens automatically when I close the sketch.

This one is fantastic. It works on so many features. Depending on the feature of choice you can select surface, plane, axis, line, vertex, point... almost anything goes though naturally depending of "the weapon of choice".

And the order in which you select these entities affects the feature. Like working with assemblies: you want two components positioned symmetrically about a face. First select the symmetry face just then the two faces that are to be symmetrically with CTRL+click and then the context toolbar should appear with options for mating... and there you will find Symmetric mate. The first selection here will determine the face that is the "midplane" in the symmetry.

[gristle]

Great add, Mark. Many thanks.

There's also an important topology lesson there. SW and the parasolid kernel hate hate HATE when things ALMOST match. The replace face trick turns an *almost* into an EXACT match.

Another version of this is to ‘move face’ the face that is almost on the centreline, then insert a cut with surface using the right (or mirror) plane.

[jcapriotti]

When I want to create an Extruded Boss/Base or Extruded Cut my usual workflow is to select the face or plane first, then the feature. That opens a sketch on the selected plane or face, and then the property manager for the feature opens automatically when I close the sketch.

This is where SolidWorks shines to me compared to other CAD tools. It's the native way it used to work, you always preselected geometry then commands, later they added the post selection. Preselection is not as intuitive for new users but the workflow is faster.

Mirror sketch is a great example, one centerline plus geometry, window select, mirror sketch button, done. I tried the same in Inventor and nothing comes close.

[Glenn Schroeder]

This is where SolidWorks shines to me compared to other CAD tools. It's the native way it used to work, you always preselected geometry then commands, later they added the post selection. Preselection is not as intuitive for new users but the workflow is faster.

Mirror sketch is a great example, one centerline plus geometry, window select, mirror sketch button, done. I tried the same in Inventor and nothing comes close.

Thank you. I use that feature extensively, but never knew you could select all the entities like that. I'll be using this workflow in the future.

If you ever get down to my part of the country I'll buy you a beer . . . or six. Maybe even supper (what some people call dinner, but I grew up with dinner being the noon meal).

[jcapriotti]

Thank you. I use that feature extensively, but never knew you could select all the entities like that. I'll be using this workflow in the future.

If you ever get down to my part of the country I'll buy you a beer . . . or six. Maybe even supper (what some people call dinner, but I grew up with dinner being the noon meal).

Just remember, you can only have one centerline, otherwise it will bring up the GUI to do the selections. With one it always skips the GUI and performs the mirror.

I'm from Mississippi so yeah, supper and dinner were the same according to my Grandma.

[CarrieIves]

This is where SolidWorks shines to me compared to other CAD tools. It's the native way it used to work, you always preselected geometry then commands, later they added the post selection. Preselection is not as intuitive for new users but the workflow is faster.

Mirror sketch is a great example, one centerline plus geometry, window select, mirror sketch button, done. I tried the same in Inventor and nothing comes close.

For the mirror in a sketch that is shown, if you are mirroring everything, you can use ctrl-a to select all. Then hit the mirror button. I put mirror on my S key because I was regularly selecting everything and mirroring.

[ellundo]

My most impressive trick was once going an entire day without a crash.
Wish I could remember how I did it.

[DennisD]

My most impressive trick was once going an entire day without a crash.
Wish I could remember how I did it.

[Glenn Schroeder]

For the mirror in a sketch that is shown, if you are mirroring everything, you can use ctrl-a to select all. Then hit the mirror button. I put mirror on my S key because I was regularly selecting everything and mirroring.

I have it as a Mouse Gesture.

image.png (26.96 KiB) Viewed 25030 times

[Lapuo]

Using format painter!
i discovered this few days ago - great help for copying dimension tolerances
(yes i know i can use styles , or pre-select and choose tolerance)
But for me this tool is most productive

[Roasted By John]

My most impressive trick was once going an entire day without a crash.
Wish I could remember how I did it.

You forgot to use the computer??

All issues with any program is "User Input" (get it?)

[mike miller]

Don't worry about it. You're not the first, and it won't be the last time. Just wait til I start spewing heresy on fully defined sketches

M'kay I'll bite.

This why underdefined sketches can be bad. Note that there is no real way to fix it without reloading the file from disk.

Under-defined Sketch.mp4

(16.6 MiB) Downloaded 406 times

[Lucas]

Not hotkeys or hidden functionality, but some tools that feels good when I use them:

Display/Delete Relations of sketch tool. Wish I knew how to use this from the very beginning, always comes in handy when there is sketch conflict, especially because some external relation gets in uninvited.

Delete Face. When you are doing some unusual geometry but the solid just keeps going through, makes a nice repair.

Also, the workflow with just one hand. I mapped S and Esc in the two additional buttons of my mouse + Mouse gestures + RBM for OK. feelsgood.jpg

[Ömür Tokman]

Select nearly anything, then hit CTRL A and it automatically filters for the type of thing that you selected and selects everything.

Want to select all edges of a part file? Select an edge, and hit CTRL A.

Want to select all faces of a part? Select a face and hit CTRL A.

Want to select all notes (and balloons) in a drawing file (in that specific sheet)? Select a note and hit CTRL A

etc....

@dpihlaja I love you Pal,
CtrlA how have I not thought of these until now.
Many shortcuts here are fine for me, but your shortcuts have been great for me.
Thank you very much for this information.

[JSculley]

Display/Delete Relations of sketch tool. Wish I knew how to use this from the very beginning, always comes in handy when there is sketch conflict, especially because some external relation gets in uninvited.

Protip: You can double-click any relation to access the Display/Delete Relations tool.

[zwei]

Using format painter!
i discovered this few days ago - great help for copying dimension tolerances
(yes i know i can use styles , or pre-select and choose tolerance)
But for me this tool is most productive

This! Never knew format painter work for tolerance...
Tried it today and work really great

[Lucas]

Protip: You can double-click any relation to access the Display/Delete Relations tool.

Good to know, thanks!

[David Matula]

when you have 3 parts that are mated together, then mated 6 to 16 other places in an assembly. Form new sub assembly, in the assembly, after mating the 3 new parts together. Them mate them to the firs place they go. Then copy with mates. When all done dissolve the sub assembly created.
Why this, cause cant use the sub assembly and dissolve it like i would like. Who says pdm and windchill are great?

[DanPihlaja]

when you have 3 parts that are mated together, then mated 6 to 16 other places in an assembly. Form new sub assembly, in the assembly, after mating the 3 new parts together. Them mate them to the firs place they go. Then copy with mates. When all done dissolve the sub assembly created.
Why this, cause cant use the sub assembly and dissolve it like i would like. Who says pdm and windchill are great?

I have no idea what you just said.......maybe some pictures?

[David Matula]

I have no idea what you just said.......maybe some pictures?

It would be like creating a bolt stack assembly that you would not be able to keep as an assembly, because of the file management system that your using. So instead of mating all the parts one at a time, you mate the parts together, and make a sub assembly in the main assembly. Then use copy with mates to mate that assembly to all the other places it goes. To insure that the programs that create the bom in the other programs work right I have to dissolve the assemblies after they have been mated.
One could attempt to pattern the assembly, but due to possible changes in parts, and trying to figure out what pattern someone created in a part in the assembly used to make the holes, it is just easier to use the copy with mates, and then if the part changes down the road, hopefully all the mates stick.

[matt]

It would be like creating a bolt stack assembly that you would not be able to keep as an assembly, because of the file management system that your using. So instead of mating all the parts one at a time, you mate the parts together, and make a sub assembly in the main assembly. Then use copy with mates to mate that assembly to all the other places it goes. To insure that the programs that create the bom in the other programs work right I have to dissolve the assemblies after they have been mated.
One could attempt to pattern the assembly, but due to possible changes in parts, and trying to figure out what pattern someone created in a part in the assembly used to make the holes, it is just easier to use the copy with mates, and then if the part changes down the road, hopefully all the mates stick.

Maybe I'm missing something, but can't you just use the Copy With Mates, but select multiple parts to copy?

[berg_lauritz]

@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.

[DennisD]

@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

Great tip!!
I've been using SWX since 1995 and never knew that (but then I mostly do R&D and don't do too many drawings anymore).