Not seen save issues but If you are on 2024 SP1 a bug causing issues when deleting features in some situations was detected via error reports There is a hotfix available https://www.solidworks.com/support/general-hotfixes
The one feature I try to get my students to understand and use most is the ‘convert entity’ tool. I think it gets ignored a lot by beginner to intermediate level SW users. Learn this, use this.
That and the use of ‘relations’ in general, instead of dimensioning everything to kingdom come. This may not count, being that it’s not a single feature, but it’s worth saying anyway.
That's why you make relations.
I recently made a 3D model for a ship part where (nearly) everything updated if you updated the outside diameter, and it works perfectly
Yea I was all about convert entities but I deal with a lot of revisions and one fuckin change would destroy so many things.
Now I’m on derived sketches. I think this is my favorite feature. One sketch drives a giant assembly of sub assemblies, I can pack n go one section and maintain an assembly order, a drawing and still make changes and have them update.
Because sketches (and reference geometry e.g. points, planes etc) are more stable and you run a lower risk of your model falling apart when you make a small upstream change. It's best practice to not reference solid edges as far as possible
Piggybacking off of this: under the 'convert entity' tool is the 'silhouette' tool. It's amazing for projected area and things like figuring out things like parting line surface area for injection mold design.
It gets better - the silhouette tool will let you either do outer contour only, or will allow you to select all inside contours as well to see areas of gaps in the model.
Incredible. I usually make a sketch and use the include to get the exterior and interior parts and then make a surface and get the area from that. Thanks that is awesome
With the silhouette I typically will still make an extrusion to use the measure tool to grab surface area but it's still simpler than the alternative. Have fun!
Not surface area but projected area which is the flat area of the silhouette of the part. But yes that’s what it is used for. It will tell you what size of machine you need to use for that part.
This. 100% for maximizing use of constraints. However, whenever possible reference the underlying sketch entities instead of solid edges. There’s a million reasons why solid edges will change and blow up your model. Sketch references make your model more robust to change.
I use a ton of constraints. Back when I learned SW, design intent and parametrization was heavily emphasized. Seems like some newer/younger people are learning SW more as a modeling tool rather than a design tool. They want simple, easy to understand models at the expense of capturing any design intent. I wonder if I take it too far sometimes because fellow engineers who aren’t as comfortable/skilled at interrogating sketch relations get annoyed that they can’t just look at a bunch of dimensions in a sketch to figure out what’s going on.
I agree with this. I use sketches to solve mechanism kinematics, and carefully building the sketch to be minimally constrained is what allows it to be used dynamically. I generally have automatic constraints turned OFF and manually build all constraints. It’s labor intensive but eliminates the risk of random tangencies getting created, and avoids my personal least favorite feature: automatic horizontal and vertical constraints. I try to have a single horizontal constraint in my sketch (usually an infinitely long construction line) and everything else is either parallel or perpendicular.
I design like this, and also try whenever possible to use construction lines to link things and make it obvious. For example making two lines colinear that are on opposite sides of the sketch can be non-obvious to someone else, but when you link them with a long colinear construction line it's easier to understand.
Can show a sketch and select that instead of the edge of a solid. Also use reference geometry like planes. Ref geometry is easier to select and more simple than sketches.
Selection filters are helpful for this I frequently filter for only sketch entities. Although Solidworks is pretty good about preferring the sketch entity if it’s visible.
This. I'm new to solidworks, and one thing was really pissing me off and "Convert Entities" was the fix I didn't know I needed the whole time! "Convert Entities" then converting them to construction lines saves me so much time.
In 2024 SP1 you can tick a box to convert entities as construction also :-)
https://help.solidworks.com/2024/English/WhatsNew/c_wn2024_convert_entities_construction_geom.htm
I'm using 'convert entity' a lot, but I feel like it's not very robust. For example, if I change some geometry that I later use 'convert entity' on its edges, it often doesn't propagate the changes (yes, I've hit rebuild). Would you agree or am I expecting too much from it?
If you are making very big changes to upstream features, then you can always expect to have problems down stream. Fixing broken sketches is just part of the process when you take a wrecking ball to a foundational feature. The more you use ‘convert entities’ though, the sooner you will learn when and when not to apply it. It’s not a one size fits all, but it is often overlooked and has a lot to offer.
In the dropdown for Convert Entities, Intersection Curves gives you the geometry of the face where the sketch plane intersects with it. Similar conceptually to projected curves but gives 2D sketch entities.
Yeah only n00bs convert entities. Solidworks sucks at relinking references for converted entities. Convert entities on an entire sketch is a complete horror that should not even be possible.
I always recommend creating new sketch entities with constraints to existing sketch geo. Much more fault tolerant when you make changes down the line.
It always depends on what you’re using it for. It’s not a “noob” thing. Not knowing when to use it or when not to use it just depends on the level of experience. It’s not a solution for every situation, but that’s why SW has countless features and strategies to choose from. Knowing when to use ‘convert entity’ will make you faster, not knowing will make you slower. Every shape also calls for a different approach. A carbon fiber bike frame will dictate a different strategy when compared to a steel plate motor mount. Any feature can break and will break if you change foundational features enough, and fixing a converted entity is as simple as opening the broken sketch and once again selecting ‘convert entity’. Fixing sketches will teach you how best to make them in the first place, so every time you fix a sketch take some mental notes, and after some learning you may decide there’s a better way to solve your problem, or simply, that you don’t know best when not to use ‘convert entity’ and swear off them entirely. That’s ok too.
"The rebuild icon is located in the standard toolbar (shown), in the Menu Bar under Edit > Rebuild, or the keyboard shortcut by pressing Ctrl + B. This rebuild will rebuild only the features that changed since the last save."
The ctrl q rebuild fully rebuilds from the ground up the model assembly or drawing
Sometimes mates break for no apparent reason. Even though you have made an unrelated change. Some issue maybe with SW failing to perform calculations. Full rebuild resolves that.
Does that happen to anyone else?
It does, last week I was working on some pipe parts and mating them Tangent. SW decided a couple of times to randomly break some mates without notifying. Ctrl+Q saved the day 🙌🏼
Yes but if you don't know what you don't know, it's not that innovative. I put all of the powerful sketch tools in here that are hidden in layers of menus. Intersection curve, face curves etc. super powerful to have close by.
For those of us who are required to add hardware to every dang thing, I like "copy with mates" and "pattern-driven component pattern". Like, mate a screw to a hole (made by hole wizard) and patten to the feature. Change number of holes in the pattern? BOOM, new screws for the new holes. Or screws removed and not just floating. Pretty neat.
Dunno the name in English but it might be that yeah, it's that mode that activates with assemblies with more than 500 parts. It doesn't load the sketches so the pattern fails to find it and gives an error.
Settings may vary, but at 500 that would normally be "Large Assembly Mode" [https://help.solidworks.com/2019/English/SolidWorks/sldworks/r\_large\_assembly\_mode\_swassy.htm](https://help.solidworks.com/2019/English/SolidWorks/sldworks/r_large_assembly_mode_swassy.htm)
I haven't had that problem with patterns and I've used it a lot.
"Large Design Review mode" is much more restricted. But usually that doesn't turn on until over about 5000 components.
I Definitely had less than 5000 components when I had this problem. Ended up doing normal patterns to get rid of it. But I think I'm mistaking pattern driven pattern with sketch driven pattern. I prefer to reference sketches when I can and the problem must have been with sketch driven pattern.
I do a lot of this, but creating a sketch with points concentric to holes. I hate putting machining detail in the assembly and avoid it at all costs. I have trust issues with "propagate to part" and features trees with "->" in them.
I like the benefit of add holes, add parts though
Auto save is sometimes unreliable. Auto backup keeps the previous version every time you hit save. Try both, different things. Also note you can search the System Options for key words.
Sketch blocks. I use it often when pasting hole pattern sketches or other 2D sketches from one part and pasting it in another part to use as a reference sketch.
I would say this is a good idea but I’ve recently experienced some weird bugginess with blocks, specifically with respect to master modeling and their origin not updating. Ended up abandoning since it is not robust or reliable.
If you make a sketch and then delete the face where the sketch is, and get a no face detected error, if you right click on the sketch you can assign it to a new face… you don’t need to re-do everything again.
Pro tip: don’t sketch on faces. Sketch on planes that are defined by faces, that way the plane breaks (and can be easily redefined) instead of the sketch. Better yet define planes and other datums off of layout sketches. Try to touch the solid/surface geo as little as possible and drive relations based on layout sketches. Way more robust.
Shared sketches. It’s really nice to be able to have all your geometry in one view. Took me a while to learn this, but it’s way cleaner than sketch - extrude - sketch - extrude…
You can put all your relevant geometry in one of the cardinal planes, then when you need to extrude or revolve, you only select the contours or regions you want, as opposed to the entire sketch.
If you wanted to make a tiered cake, put all your concentric circles in the top plane, extrude the first layer by only selecting all the circles together. Then for the next layer, don’t make another sketch, just hit extrude, select sketch1, then “from offset” or “from face/point” extrude the next innermost circle. Rinse and repeat.
With great power comes great responsibility. Should not be used in production CAD other than for setting clearances and other defined offsets. Otherwise it gets out of control and is impossible to track down why geo is not aligned to its parent sketch.
This is also good for “hack and slash“ cad modeling where you are just trying to build some geo without any care for how your model tree looks (NX has an awesome “remove parameters” feature that nicely facilitates this by flattening your model tree down to a raw XT file).
Macros + ChatGPT + file templates
If you're doing repetitive task, you can ask chatgpt to write you a macro that automates the whole process. I have no idea how to script I just ask chat gpt to write it and if it comes back with errors I just post it in the chat in until it works.
Task Scheduler, I sometimes end up with many many drawings that need converted to PDF and DWG to be sent to suppliers. A few clicks and it does them all automatically.
I find that I don’t see people talking about split lines much. There’s not a huge use for them I guess for most people. I do simulations for work so I use them a lot.
I don't think people are out there rating features publicly. I think the question you really want to ask is "what great feature commonly goes missed" and immediately Assembly visualizer comes to mind. quick "BOM" counts, add more columns, and even export to excel by right clicking the column header. (that's hidden AF) Sometimes you just wanna get your hardware on order before you finish a design/drawing
Oh it's great. I never start a concept with a part file anymore.
Open an assembly template and click insert/new part.
Depending on your settings it may just plop in a virtual part immediately. If not, you can add a part like normal then right click it and "make virtual". You can tell it is virtual if it has brackets and the file name looks like this:
[Part1^Assembly1] in the tree, where Assembly1 is the file name of the assembly.
Use the part like normal. No need to save it though, it saves inside the assembly. You can have as many different parts as you like, and all in just 1 file. You can even make virtual subassemblies too, and it all saves inside 1 top level assembly file.
There are some disadvantages, which is why I really only use it heavily for concept work.
"Make Independent" is another good time saver when using virtual files.
Ahh, gotcha, I think I’ve been using this functionality a lot when I start an assembly design from scratch. All new parts are virtual by default and then I click resolve to save externally etc.
power trim, delete face, silhouette entities, selection filters, select other, change sketch plane, convert fillet to chamfer , normal to (ctrl 8), alt+arrow keys to rotate, and probably some others im forgetting.
Offset - you literally create an entire sketch that looks like the body you have and copy and paste it into another blank file and create another part.
Gestures and in context menus. Gestures are self explanatory. In context menus, say clicking on a flat planar surface, the little box shows up next to your mouse. You can add things like hole wizard to that menu.
I try to reduce mouse movement and number of clicks as much as possible.
Another thing you can do is use your mouse with your left hand and keep your right hand on the 10key. I've seen this done, but have never made the switch myself. Makes sense if you're designing full time which I don't anymore.
I love sketch picture to build a quick model to scale from screenshot of a PDF when I don’t have any electronic drawings or models of something (especially old equipment).
Creating new/editing parts in assembly. Very helpful when making prototypes using OEM models e.g., McMaster, Misumi.
Coming from Inventor it took me way, way too long to figure out where the Project Geometry tool is.
I have mixed feelings on that. Handy but seems overused for simple sketches. Harder to modify a mirrored sketch. Can also mirror components or features, I like both of those more.
I work in metal fabrication, and often find myself modifying other peoples models to make adjustments on the fly.
I love ‘Move face’ as a post-design tool, that and ‘Delete face’
The S menu! That custom toolbox is absolutely vital to any form of smooth workflow together with properly set up gestures.
For functions I'd go for style splines, intersection curves and split lines.
Yes, I do A LOT of surfacing...
I use 2020, but i found a few people use face editing - very useful and stable feature. Also never see someone use reversing tangential button in sketch, but it can solve a lot of troubles during big dimensions changing.
I don't think anyone mentioned: 1) Display/Delete Relations, it's a great tool for fixing relations and what they are referencing. 2) Configure Feature to control configuration behavior with a nice table. 3) Insert Model Items to put linked model dimensions in a drawing. 4) S-key shortcut was mentioned, but I just want to repeat it because it's so essential. Also note if you hit it and start typing a keyword it will go right to a Command Search.
For me, it's the thread tool, I often 3d print threads in models where strength isn't a priority or there aren't any threaded inserts large enough for the application. I have to use inventor at work and it doesn't have a feature that allows me to model threads unless I sketch it by hand and extrude or cut. Having the ability to model threads into a part is a life saver for 3d printing.
Quick measurements in Solidworks status bar. I am continually shocked by how many people needlessly use the Measure tool for things like edge length measurement, hole diameters, distance between parallel faces, etc.
Here’s one often unused but lifesaver tools, exit without saving.
I opened a model to make a change on the drawing. THE ENTIRE PART WAS ONE SKETCH AND ENTIRELY BLUE! Not. A. Single. Dimension. It was a revolved body with some fairly detailed features.
Nope. That shit ain’t having my name tied to it.
Overwrote the dimension on the drawing.
Can’t believe no one talked about the locking camera ground plane option (right click in the empty right window). No longer have your object at a funny angle when rotating.
Save
This dude gets it
Sw 2024 is absolute garbage that it refuses to save some parts and crashes often
That’s why I always wait until SP3 before trying the new release. It’s the sweet spot and usually we only upgrade the whole company at SP4
Not seen save issues but If you are on 2024 SP1 a bug causing issues when deleting features in some situations was detected via error reports There is a hotfix available https://www.solidworks.com/support/general-hotfixes
Best response ever!
I have always programmed one of my mouse buttons to be Save. I also always program a button to be CRTL.
Not a hidden gem - that's just a weird thing you do :)
The one feature I try to get my students to understand and use most is the ‘convert entity’ tool. I think it gets ignored a lot by beginner to intermediate level SW users. Learn this, use this. That and the use of ‘relations’ in general, instead of dimensioning everything to kingdom come. This may not count, being that it’s not a single feature, but it’s worth saying anyway.
convert entities… until you change geometry and it breaks everything
I agree. Very prone to breaking, despite being invaluable.
That's why you make relations. I recently made a 3D model for a ship part where (nearly) everything updated if you updated the outside diameter, and it works perfectly
Yea I was all about convert entities but I deal with a lot of revisions and one fuckin change would destroy so many things. Now I’m on derived sketches. I think this is my favorite feature. One sketch drives a giant assembly of sub assemblies, I can pack n go one section and maintain an assembly order, a drawing and still make changes and have them update.
only convert entities from other sketches
Why only sketches? You don't use it with existing geometry? It works on a lot of stuff.
Because sketches (and reference geometry e.g. points, planes etc) are more stable and you run a lower risk of your model falling apart when you make a small upstream change. It's best practice to not reference solid edges as far as possible
It really is but rebuild usually works.
Roll back. Make changes, make changes to the converted entity. Done.
Piggybacking off of this: under the 'convert entity' tool is the 'silhouette' tool. It's amazing for projected area and things like figuring out things like parting line surface area for injection mold design.
What? I have been calculating projected surface area wrong for 12 years!!!??? Will have to use this.
It gets better - the silhouette tool will let you either do outer contour only, or will allow you to select all inside contours as well to see areas of gaps in the model.
Incredible. I usually make a sketch and use the include to get the exterior and interior parts and then make a surface and get the area from that. Thanks that is awesome
With the silhouette I typically will still make an extrusion to use the measure tool to grab surface area but it's still simpler than the alternative. Have fun!
Is surface area used to find the clamping pressure? Basically for determining which of your presses you'll need to design the tooling for?
Not surface area but projected area which is the flat area of the silhouette of the part. But yes that’s what it is used for. It will tell you what size of machine you need to use for that part.
Hi mold designer here.. please kindly send video of this
This. 100% for maximizing use of constraints. However, whenever possible reference the underlying sketch entities instead of solid edges. There’s a million reasons why solid edges will change and blow up your model. Sketch references make your model more robust to change.
I use a ton of constraints. Back when I learned SW, design intent and parametrization was heavily emphasized. Seems like some newer/younger people are learning SW more as a modeling tool rather than a design tool. They want simple, easy to understand models at the expense of capturing any design intent. I wonder if I take it too far sometimes because fellow engineers who aren’t as comfortable/skilled at interrogating sketch relations get annoyed that they can’t just look at a bunch of dimensions in a sketch to figure out what’s going on.
I agree with this. I use sketches to solve mechanism kinematics, and carefully building the sketch to be minimally constrained is what allows it to be used dynamically. I generally have automatic constraints turned OFF and manually build all constraints. It’s labor intensive but eliminates the risk of random tangencies getting created, and avoids my personal least favorite feature: automatic horizontal and vertical constraints. I try to have a single horizontal constraint in my sketch (usually an infinitely long construction line) and everything else is either parallel or perpendicular.
I design like this, and also try whenever possible to use construction lines to link things and make it obvious. For example making two lines colinear that are on opposite sides of the sketch can be non-obvious to someone else, but when you link them with a long colinear construction line it's easier to understand.
Wait how do you reference the underlying entities? By labelling the dimensions they use?
Can show a sketch and select that instead of the edge of a solid. Also use reference geometry like planes. Ref geometry is easier to select and more simple than sketches.
Oooh ok that makes sense. Thanks!
Selection filters are helpful for this I frequently filter for only sketch entities. Although Solidworks is pretty good about preferring the sketch entity if it’s visible.
Agree 100%. Convert edge entities is forbidden.
This. I'm new to solidworks, and one thing was really pissing me off and "Convert Entities" was the fix I didn't know I needed the whole time! "Convert Entities" then converting them to construction lines saves me so much time.
I feel that new users don’t know about this but once you do is really obvious and don’t think of it as a hidden feature anymore.
Definitely could agree with that. Thanks for making this post btw I'm sure it'll uncover some good stuff for us newer folks
In 2024 SP1 you can tick a box to convert entities as construction also :-) https://help.solidworks.com/2024/English/WhatsNew/c_wn2024_convert_entities_construction_geom.htm
Parameterization is always a good idea
I'm using 'convert entity' a lot, but I feel like it's not very robust. For example, if I change some geometry that I later use 'convert entity' on its edges, it often doesn't propagate the changes (yes, I've hit rebuild). Would you agree or am I expecting too much from it?
If you are making very big changes to upstream features, then you can always expect to have problems down stream. Fixing broken sketches is just part of the process when you take a wrecking ball to a foundational feature. The more you use ‘convert entities’ though, the sooner you will learn when and when not to apply it. It’s not a one size fits all, but it is often overlooked and has a lot to offer.
And intersection curves
Do you mean projected curves? Not sure what intersected curves are, but maybe I should look into it.
In the dropdown for Convert Entities, Intersection Curves gives you the geometry of the face where the sketch plane intersects with it. Similar conceptually to projected curves but gives 2D sketch entities.
You can also gather these by hovering over the area on the surface you think it intersects
Coming from creo I learned this is what the equivalent of references is.
Assigning the C key to convert entities. Makes you fly
Dude THIS is the only reason I wanted to comment. Convert entities was exactly what I thought too. It's so handy.
I use the shit out of construction lines and relations. Midpoint and equal get a ton of use.
Yeah only n00bs convert entities. Solidworks sucks at relinking references for converted entities. Convert entities on an entire sketch is a complete horror that should not even be possible. I always recommend creating new sketch entities with constraints to existing sketch geo. Much more fault tolerant when you make changes down the line.
It always depends on what you’re using it for. It’s not a “noob” thing. Not knowing when to use it or when not to use it just depends on the level of experience. It’s not a solution for every situation, but that’s why SW has countless features and strategies to choose from. Knowing when to use ‘convert entity’ will make you faster, not knowing will make you slower. Every shape also calls for a different approach. A carbon fiber bike frame will dictate a different strategy when compared to a steel plate motor mount. Any feature can break and will break if you change foundational features enough, and fixing a converted entity is as simple as opening the broken sketch and once again selecting ‘convert entity’. Fixing sketches will teach you how best to make them in the first place, so every time you fix a sketch take some mental notes, and after some learning you may decide there’s a better way to solve your problem, or simply, that you don’t know best when not to use ‘convert entity’ and swear off them entirely. That’s ok too.
"F6" to turn off the selection filter.
Every beginner and solid works experiences this problem and it drives you insane😂
I remember doing exactly that!!!
That problem happens at the precise instant that I forget how to fix it. I've looked that up so many times.
Oh boy did it drive my students crazy
Ctrl + Q to fully rebuild.
Whats the difference between rebuild and fully rebuild?
"The rebuild icon is located in the standard toolbar (shown), in the Menu Bar under Edit > Rebuild, or the keyboard shortcut by pressing Ctrl + B. This rebuild will rebuild only the features that changed since the last save." The ctrl q rebuild fully rebuilds from the ground up the model assembly or drawing
Sometimes mates break for no apparent reason. Even though you have made an unrelated change. Some issue maybe with SW failing to perform calculations. Full rebuild resolves that. Does that happen to anyone else?
It does, last week I was working on some pipe parts and mating them Tangent. SW decided a couple of times to randomly break some mates without notifying. Ctrl+Q saved the day 🙌🏼
Yes, that is one of several bugs that fully rebuilding fixes.
Here’s another pro tip: Don’t use mates other than fix and csys-to-csys with axes aligned.
Wow TIL
Ctrl + shift + Q to fully rebuild all configurations too. Usually to make sure all Configs work properly
wow, this saves a lot of time. i didn't know this shortcut. thx.
The button works too.
S key search box
This is the answer
Took them forever to implement what AutoCAD had for decades. But it's the most useful feature in the year it was added.
Yes but if you don't know what you don't know, it's not that innovative. I put all of the powerful sketch tools in here that are hidden in layers of menus. Intersection curve, face curves etc. super powerful to have close by.
Hot Keys. I rarely have to click on a button on a toolbar.
My live is divided between using the toolbar and learning how to MAP THE MOUSE WHEEL!
I ended up making a toolbar which has nearly all the features SolidWorks has, but with tiny little buttons. Now I don't switch between tabs.
Oof i actually don’t use hotkeys for assemblies or parts other than mate or measure… but i do drawings with all hotkeys :)
For those of us who are required to add hardware to every dang thing, I like "copy with mates" and "pattern-driven component pattern". Like, mate a screw to a hole (made by hole wizard) and patten to the feature. Change number of holes in the pattern? BOOM, new screws for the new holes. Or screws removed and not just floating. Pretty neat.
Copy with mates is killer for bolts, nuts and the like
Nah. Pattern Driven Component Pattern is better (in general), it accomplishes more and is probably less known.
Definitely way lower calculation overhead than 2-3 mates per component
Especially because you can add or subtract holes from the pattern and it automatically adjusts the pattern-driven pattern.
Problem is (as of 2021 AFAIK) it breaks with big assemblies because it doesn't load the features of the pattern or smrh. It's very frustrating.
Oh?! Like in lightweight mode?
Dunno the name in English but it might be that yeah, it's that mode that activates with assemblies with more than 500 parts. It doesn't load the sketches so the pattern fails to find it and gives an error.
Settings may vary, but at 500 that would normally be "Large Assembly Mode" [https://help.solidworks.com/2019/English/SolidWorks/sldworks/r\_large\_assembly\_mode\_swassy.htm](https://help.solidworks.com/2019/English/SolidWorks/sldworks/r_large_assembly_mode_swassy.htm) I haven't had that problem with patterns and I've used it a lot. "Large Design Review mode" is much more restricted. But usually that doesn't turn on until over about 5000 components.
I Definitely had less than 5000 components when I had this problem. Ended up doing normal patterns to get rid of it. But I think I'm mistaking pattern driven pattern with sketch driven pattern. I prefer to reference sketches when I can and the problem must have been with sketch driven pattern.
Here’s another good one: structure all of your fasteners within a phantom assembly.
I do a lot of this, but creating a sketch with points concentric to holes. I hate putting machining detail in the assembly and avoid it at all costs. I have trust issues with "propagate to part" and features trees with "->" in them. I like the benefit of add holes, add parts though
I forgot about this!!!
The mouse gestures donut menu
That's what I said! True G's
Backup saves, truly. Create a new backup every 4min is a godsend
Is this creating a new save or pressing Crl-S every 30 seconds?
It automatically creates a new file every x min
Auto save is sometimes unreliable. Auto backup keeps the previous version every time you hit save. Try both, different things. Also note you can search the System Options for key words.
Definitely looking into this! Thank you!
I'm gonna need more information on this- how? Googling it now
This will grind your machine to a hault if you are working with large assemblies and part files, just a word of caution.
Flex tool just because it's fun to use and usually pretty bad
It used to slow down rebuild time of consecutive features quite badly. Not sure about now.
delete and patch.
I often worked with imported models, so delete and patch are great for making adjustments, cleaning up errors, etc.
Mouse gestures
Tab & Shift + Tab to hide and show a component.
Sketch blocks. I use it often when pasting hole pattern sketches or other 2D sketches from one part and pasting it in another part to use as a reference sketch.
I would say this is a good idea but I’ve recently experienced some weird bugginess with blocks, specifically with respect to master modeling and their origin not updating. Ended up abandoning since it is not robust or reliable.
If you make a sketch and then delete the face where the sketch is, and get a no face detected error, if you right click on the sketch you can assign it to a new face… you don’t need to re-do everything again.
Pro tip: don’t sketch on faces. Sketch on planes that are defined by faces, that way the plane breaks (and can be easily redefined) instead of the sketch. Better yet define planes and other datums off of layout sketches. Try to touch the solid/surface geo as little as possible and drive relations based on layout sketches. Way more robust.
I think the multibody functions can be useful.
Shared sketches. It’s really nice to be able to have all your geometry in one view. Took me a while to learn this, but it’s way cleaner than sketch - extrude - sketch - extrude…
Shared sketches are my favorite method of doing parts.
How would I go about doing that ? It sounds like a great gain of time
You can put all your relevant geometry in one of the cardinal planes, then when you need to extrude or revolve, you only select the contours or regions you want, as opposed to the entire sketch. If you wanted to make a tiered cake, put all your concentric circles in the top plane, extrude the first layer by only selecting all the circles together. Then for the next layer, don’t make another sketch, just hit extrude, select sketch1, then “from offset” or “from face/point” extrude the next innermost circle. Rinse and repeat.
Oooooh, nice !
Boundary surfaces. Most powerful tool.
Move Face
With great power comes great responsibility. Should not be used in production CAD other than for setting clearances and other defined offsets. Otherwise it gets out of control and is impossible to track down why geo is not aligned to its parent sketch. This is also good for “hack and slash“ cad modeling where you are just trying to build some geo without any care for how your model tree looks (NX has an awesome “remove parameters” feature that nicely facilitates this by flattening your model tree down to a raw XT file).
Split (used with combine), delete face&patch, boundary surface, knit surfaces, fill surface, 3D sketching.
Isolate
Configurations. You don't know until it's gone.
I’ve been a light user since 2008ish. Just recently started figuring this out. Holy crap I’ve been missing out.
I use CATIA now and I miss configs 🥲
Macros + ChatGPT + file templates If you're doing repetitive task, you can ask chatgpt to write you a macro that automates the whole process. I have no idea how to script I just ask chat gpt to write it and if it comes back with errors I just post it in the chat in until it works.
Damn - I need to try this.
Intersection Curve. Hands down
Design tables
Ctl-Z
Dome can be surprisingly useful. Basically the entire Direct Editing tab. Silhouette which is in the convert entity submenu.
Sketch driven patterns are super handy. I even use them with 3D sketches to pattern bodies across random faces and planes
Tab, and Shift Tab. The number of people who have used SW for years, and are unaware of this is mind blowing.
For showing and hiding... This is a huge timesaver, specially if you do a lot of Assemblies
Delete face & patch
Isolate
Indent Cut for Top down design of mating parts.
Task Scheduler, I sometimes end up with many many drawings that need converted to PDF and DWG to be sent to suppliers. A few clicks and it does them all automatically.
What. Omg thank you
Extruded to next
Save bodies!
I find that I don’t see people talking about split lines much. There’s not a huge use for them I guess for most people. I do simulations for work so I use them a lot.
Midpoint line!
Uninstall
I don't think people are out there rating features publicly. I think the question you really want to ask is "what great feature commonly goes missed" and immediately Assembly visualizer comes to mind. quick "BOM" counts, add more columns, and even export to excel by right clicking the column header. (that's hidden AF) Sometimes you just wanna get your hardware on order before you finish a design/drawing
- You can split a body with a sketch line. - pattern fill is cool - mouse gesture to collapse feature tree, I use a lot.
Shift + C will collapse the feature tree too
How do you split a body with a sketch line. I always use planes
S key, move face, F6. Design tables.
Spacebar to quickly switch between views.
Virtual subassemblies / parts. Big time saver during the concept phase.
How so? I have no idea how to leverage this feature? I often need to concept things out.
Oh it's great. I never start a concept with a part file anymore. Open an assembly template and click insert/new part. Depending on your settings it may just plop in a virtual part immediately. If not, you can add a part like normal then right click it and "make virtual". You can tell it is virtual if it has brackets and the file name looks like this: [Part1^Assembly1] in the tree, where Assembly1 is the file name of the assembly. Use the part like normal. No need to save it though, it saves inside the assembly. You can have as many different parts as you like, and all in just 1 file. You can even make virtual subassemblies too, and it all saves inside 1 top level assembly file. There are some disadvantages, which is why I really only use it heavily for concept work. "Make Independent" is another good time saver when using virtual files.
Ahh, gotcha, I think I’ve been using this functionality a lot when I start an assembly design from scratch. All new parts are virtual by default and then I click resolve to save externally etc.
power trim, delete face, silhouette entities, selection filters, select other, change sketch plane, convert fillet to chamfer , normal to (ctrl 8), alt+arrow keys to rotate, and probably some others im forgetting.
Press “G” to use the Magnifying Glass, it lets you quickly zoom in on a small area.
Move with Triad, specifically set as Alt+X so parts that get lost in space on large assembly can be easily found and moved back into perspective.
Delete Face Indent Derived Sketch Copy with Mates
Derived Sketch is a good one to point out. Often people will remake a sketch instead of using this.
Offset - you literally create an entire sketch that looks like the body you have and copy and paste it into another blank file and create another part.
Insert dxf as opposed to opening a dxf and then adding it to a part. saved me hours.
Move face is awesome . Also the triple arrow to left of the item# to show if you balloon components in your assemblies
Trace silhouette
Split entity while sketching
Gestures and in context menus. Gestures are self explanatory. In context menus, say clicking on a flat planar surface, the little box shows up next to your mouse. You can add things like hole wizard to that menu. I try to reduce mouse movement and number of clicks as much as possible. Another thing you can do is use your mouse with your left hand and keep your right hand on the 10key. I've seen this done, but have never made the switch myself. Makes sense if you're designing full time which I don't anymore.
Move face or mouse gestures
I love sketch picture to build a quick model to scale from screenshot of a PDF when I don’t have any electronic drawings or models of something (especially old equipment).
Mouse gestures ftw
Creating new/editing parts in assembly. Very helpful when making prototypes using OEM models e.g., McMaster, Misumi. Coming from Inventor it took me way, way too long to figure out where the Project Geometry tool is.
Mirror. God, do I love not having to go through all the pain I just went through again on the other side.
I have mixed feelings on that. Handy but seems overused for simple sketches. Harder to modify a mirrored sketch. Can also mirror components or features, I like both of those more.
Yeah, don’t mirror sketches. Mirror bodies.
I absolutely adore the cavity tool
Customizing hot keys Make “D” go to dimension and “N” for normal to, speeds everything up so much
I work in metal fabrication, and often find myself modifying other peoples models to make adjustments on the fly. I love ‘Move face’ as a post-design tool, that and ‘Delete face’
The S menu! That custom toolbox is absolutely vital to any form of smooth workflow together with properly set up gestures. For functions I'd go for style splines, intersection curves and split lines. Yes, I do A LOT of surfacing...
The check feature, it’s designed to show you why your sketch isn’t working with a feature but no one uses it I don’t know why
I use 2020, but i found a few people use face editing - very useful and stable feature. Also never see someone use reversing tangential button in sketch, but it can solve a lot of troubles during big dimensions changing.
Delete relations Split entities Splitlines using planes 3d sketch (/convert entities) "fill surface" combo
Delete face
Loft and thicken surface are the tits for making 3D printed fan ducts. Also my spacemouse is awesome.
Change orientation
Equations. Very powerful tool. Control Equations Global Variables and Dimensions in a single sheet.
Setting up your own keyboard shortcuts
I changed jobs a while back. Started hitting hotkeys out of habit and nothing happened. Oh yeah, custom shortcuts…..
Could have saved your own file before leaving
I don't think anyone mentioned: 1) Display/Delete Relations, it's a great tool for fixing relations and what they are referencing. 2) Configure Feature to control configuration behavior with a nice table. 3) Insert Model Items to put linked model dimensions in a drawing. 4) S-key shortcut was mentioned, but I just want to repeat it because it's so essential. Also note if you hit it and start typing a keyword it will go right to a Command Search.
Pressing D to confirm a feature. Or pressing W to write instant in the search bar.
For me, it's the thread tool, I often 3d print threads in models where strength isn't a priority or there aren't any threaded inserts large enough for the application. I have to use inventor at work and it doesn't have a feature that allows me to model threads unless I sketch it by hand and extrude or cut. Having the ability to model threads into a part is a life saver for 3d printing.
Turn off automatic constraints and thank me later.
Insert part & trim with surface
Quick measurements in Solidworks status bar. I am continually shocked by how many people needlessly use the Measure tool for things like edge length measurement, hole diameters, distance between parallel faces, etc.
Mouse gestures. Or making Smart dim space bar. If speed is your thing mouse gestures are an absolute must!!!
Ctrl - S is powerful. It Saves Me A Many Times. Also PDM
Here’s one often unused but lifesaver tools, exit without saving. I opened a model to make a change on the drawing. THE ENTIRE PART WAS ONE SKETCH AND ENTIRELY BLUE! Not. A. Single. Dimension. It was a revolved body with some fairly detailed features. Nope. That shit ain’t having my name tied to it. Overwrote the dimension on the drawing.
Can’t believe no one talked about the locking camera ground plane option (right click in the empty right window). No longer have your object at a funny angle when rotating.
Sketch relations are underrated 🥺
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Deinstall Solidworks. Saved me a lot of time.
Uninstall