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    Default SOLIDWORKS Tips & Tricks

    I thought I would start a thread featuring SW users' favorite timesavers, work-arounds, etc.

    I'll start with a few basic ones:

    Use Ctrl+Tab to switch between SW windows.
    Use the "F" key for zoom-to-fit when you bump your mouse and the model disappears.
    Make your own easy to remember hot-keys for often repeated commands. (I use this a LOT.{Save-as, open, close, wireframe view, shaded view, new asm. from part, etc.})
    Customize mouse gestures and USE THEM!
    Double-click inside a sketch to accept and exit.
    Use relations as much as possible in sketches for better design intent.
    Use your "S" hot key for quick commands.
    The linear pattern feature can skip and vary instances for erratic spacing.
    Use the revolve feature for "roundish" parts. You can do most of the part with only one feature vs. various extrudes and cuts.

    Feel free to add to this. We can all learn new shortcuts.


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    Thanks for sharing ChipSplitter, I'll add a couple that prove useful to me...
    - Use blocks to save/transfer 2D design content. Downside is that it doesn't update. Upside is that is doesn't update
    - I like insert -> part to create parts that are linked in a parent-child format. The child part will update with changes to the parent (imported) part.
    - Take the time to set up templates for your part/assembly/drawings
    - Don't update all the time. Find a consistent package for your workflow and hardware and stick with it

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    In a revolve, draw a construction line for your part center and dimension from it.if you drag your dimension down past the construction line it will go from the radius of the part to full diameter.



    Sent from my Pixel 3 using Tapatalk

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    Quote Originally Posted by as9100d View Post
    In a revolve, draw a construction line for your part center and dimension from it.if you drag your dimension down past the construction line it will go from the radius of the part to fill diameter.



    Sent from my Pixel 3 using Tapatalk
    Aha......neat!

    I never discovered that.

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    When entering values for dimensions, you can use standard arithmetic like an excel cell. This helps not pull up the calculator all the time.

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    Here's a few more:

    -When doing complex parts with a long FeatureTree rename all the features to keep track of them, i.e. Main Base BE (BE for Boss-Extrude), Big Hole CE (Cut-Extrude).
    That way you can use the search field at the top of the FeatureManager to find all Boss-Extrudes, for example.
    - Use folders for families of parts and mates in assemblies. I put all fasteners in one folder, for example.
    -Learn to utilize equations (I'm just learning this ). Especially nice when working with families of parts.
    -Use the reload function when you go down a bunny trail and majorly screw something up (you guys of course never do this ). It automatically closes the file w/o saving and reopens.
    - "R" key opens the Welcome dialog with up to 100 recent files. You can also pin files and folders so they are always there.

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    Another big one I learned from Motion Guru. In an assembly, double click on a feature to bring up the sketch driving it. Then you can modify dimensions and rebuild to have the changes take effect. You gotta be careful with mates though. This can blow them up quickly if you aren't careful.

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    Get yourself a useful mouse with at least fwd/back buttons and remap them to enter and esc. Super useful and saves incredible amount of time. I use a Logitech MX Master and their options software, but can be done with any mouse and "X-Mouse Button Control" software.

    I write a ton of custom hotkeys for views like isometric (ctrl+E) and normal to (crtl+D), change a bunch of sketch functions to things that I can remember like "L" for line, "C" for circle etc.

    Learn your right click menus and what is there during different tasks, keeps you from fumbling thru the ever changing top bar menus.

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    Quote Originally Posted by BugRobotics View Post
    Don't update all the time. Find a consistent package for your workflow and hardware and stick with it
    Best piece of SW advice EVER. Stick to what you're fast and effective with. I have yet to find anything I can't do with SW 2014. I pay the annual maintenance but don't install the annual updates. Why waste time learning new icons and menus? They take away as much functionality as they add, and Time is Money.

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    2016 is my jam...

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    I froze everything, including the OS, at 2014 because that's the last edition of Adobe Creative Suite (and some other things like Mastercam) you could actually own.

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    If you have solid works set to inches, you can dimension in millimetres by typing mm after the dimension and solid works will automatically convert to inches. Obviously the reverse work as well.

    EX, type 30mm -> 1.1811

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    Re-posting a reply I made about a 4th axis path on a cylinder if somebody missed it. Images won't open for larger view, find original reply in CAD-CAM forum. SolidQuirks 2014 used.


    A swept profile cut may work unless the amount of twist is too great. That seems to depend upon how far around the cylinder you're going. You can create a path or a slot on a plane and project it on the cylinder face, there may limitations to this as well. You can create a 3D sketch by using the "convert" call for extruding the cut but the ends of the profile will be affected by the vector direction you choose. This may work fine if you work in short sections and attach/merge one to another. I've not tried to create an entire drum with the shift paths but I tried using a loft cut long enough to find the failure point. The profiles and the path need to intersect at some point, a "Pierce" constraint may be needed, depending upon whether you're using a sweep, extrude, or loft. Once you select the closed profiles (Two or more) you use the projected/wrapped curve as a "Centerline Parameter" rather than a "Guide Curve". Pick the same corner point in each profile (Upper Left - Upper Left for eg.) or the loft will rotate accordingly. It may/may not work for what you're doing, I'll leave that for you to determine. Seemed to leave parallel walls and not twist to the profile. The images are below, hope this helped.

    drum-over.jpg

    drum-x-sect.jpg

    drum-over2.jpg

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    Quote Originally Posted by kenton View Post
    If you have solid works set to inches, you can dimension in millimetres by typing mm after the dimension and solid works will automatically convert to inches. Obviously the reverse work as well.

    EX, type 30mm -> 1.1811
    You can also mix and match when doing math, typing "12.7mm + .5in" will get 1 inch.

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    Quote Originally Posted by EOLSON View Post
    Get yourself a useful mouse with at least fwd/back buttons and remap them to enter and esc. Super useful and saves incredible amount of time. I use a Logitech MX Master and their options software, but can be done with any mouse and "X-Mouse Button Control" software.

    I write a ton of custom hotkeys for views like isometric (ctrl+E) and normal to (crtl+D), change a bunch of sketch functions to things that I can remember like "L" for line, "C" for circle etc.

    Learn your right click menus and what is there during different tasks, keeps you from fumbling thru the ever changing top bar menus.
    I use the MX Master as well. I really like it, but with 3 programmable buttons plus 4 gestures plus my 8 SW mouse gestures I get a bit overwhelmed with options....
    I did remap my fwd/back buttons once, but it drove me nuts when I was using File Explorer and jumping between folders. Whatever works best for you, I guess.
    My number one favorite thing about SW is the level of user customization there is for commands.
    The only downside is if I were to jump on one of you guys' computer I would be lost instantly.

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    Another quick tip is to turn on dynamic relationships in parts to show what features are influencing other features. Helpful to track down issues when your feature tree starts to get larger.

    Here's what it looks like in action...

    dynamic-relationships.jpg

    To turn on, right click on the part name in the feature tree and click the two buttons highlighted yellow in the image below.

    dynamic-relationships-1.jpg

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    Quote Originally Posted by BugRobotics View Post
    Another quick tip is to turn on dynamic relationships...
    I have wanted this for the last 9 years! I hate digging back through sketches to find something snapped to the midpoint of a line which happens to be at the origin.

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    Quote Originally Posted by BugRobotics View Post
    Another quick tip is to turn on dynamic relationships in parts to show what features are influencing other features. Helpful to track down issues when your feature tree starts to get larger.

    Here's what it looks like in action...

    dynamic-relationships.jpg

    To turn on, right click on the part name in the feature tree and click the two buttons highlighted yellow in the image below.

    dynamic-relationships-1.jpg
    Oh man, this one is awesome. Thanks for sharing!

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    Quote Originally Posted by BugRobotics View Post
    Another quick tip is to turn on dynamic relationships in parts to show what features are influencing other features. Helpful to track down issues when your feature tree starts to get larger.

    Here's what it looks like in action...

    dynamic-relationships.jpg

    To turn on, right click on the part name in the feature tree and click the two buttons highlighted yellow in the image below.

    dynamic-relationships-1.jpg
    SUPER!
    You should get the "Engineer of the Year" award for that one.

    There are so many times when I want to delete a part and can't figure out what children it has.

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    here are a bunch of training and tips and trick from a former coworker (92-93) and SW employee.

    I worked with him at IDEO, he was a Industrial Designer and I was one of the model makers,
    he then went on to SW to help improve the surfacing stuff, now he is back designing and created these vids.

    I have been at a couple of his breakout sessions at SW-World over the years too.

    tricks I use alot is move face, replace face, contour select, master model, control 1-7 (views), create my own views when imported parts are wonky (hit space bar to get it), part in part and alot of configurations of parts for CAM work.



    SolidWorks Tips and Techniques Video Series

    Discussion created by Mark Biasotti on Mar 17, 2020
    Latest reply on May 29, 2020 by Renee Kontra



    So, what are you doing with your time right now? If you are like me you are in "shelter-in" mode (most of the Bay Area is in Covid-19 lock-down mode) trying to do my work from home in close quarters 24/7 with my wife and golden retriever - a weird new normal...

    So with the disruption and perhaps some time on your hands, it might be good timing to release the first eight episodes of our Spanner Tips and Techniques Webcasts. Its an all-things product design video series focusing industry methods and practices that we employ here at Spanner every day. We're starting off the webcast series with our SolidWorks Tips and Techniques series. The first 8 episodes are live and you can view them by visiting our website here:

    Webcasts — Spanner Product Development

    I plan on doing approximately two dozen episodes pertaining to SolidWorks. These are focused on Consumer product design in SolidWorks but I'm sure there is something for everyone. I'm currently working on the next few episodes and will be adding one per week or so.

    Follow us on the Spanner Tips and Techniques | SolidWorks Webcast - YouTube playlist

    Following is an agenda of what is posted and what is to come:

    1. SolidWorks Tips and Techniques Part 1 – 8 tips and tricks for SW users to improve their productivity and modeling quality.
    2. SolidWorks Tips and Techniques Part 2 – 8 tips and tricks for SW users to improve their productivity and modeling quality.
    3. SolidWorks Tips and Techniques Part 3 – 8 tips and tricks for SW users to improve their productivity and modeling quality.
    4. Making bullet-proof models – robustly and efficiently for parametric change
    5. Advanced Modeling Part 1 – What is advanced modeling and how is it different
    6. Advanced Modeling part 2 – Working with Curves
    7. Advanced Modeling Part 3 – more Working with Curves
    8. Advanced Modeling Part 3 – Working between Solids and Surfaces
    9. Advanced Modeling Part 4 – Boundary Surface techniques
    10. Advanced Modeling Part 5 – more Boundary surface
    11. Advanced Modeling Part 6 - Fill Surface
    12. Advanced Modeling Part 8 - sweep techniques
    13. Advanced Modeling Part 9 – All about the Flex Feature
    14. Advance Modeling Part 10 – working with fillets
    15. Advance Modeling Part 11 – more fillets
    16. Advanced Modeling Part 12 – Deform Freeform features explained
    17. Advanced Modeling Part 13 - Master Model Technique Part 1
    18. Advanced Modeling Part 14 - Master Model Technique continued
    19. Advanced Modeling Part 15 - Delete, Replace, Move, Heal Face.
    20. Engineers and Industrial Designers Working together Part 1 – how to successfully work together to faithfully capture and reproduce design intent.
    21. Cross-Platform collaboration between SolidWorks and other CAD
    22. More SolidWorks Tip and Tricks – Part 4


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