What are your most impressive tricks of solidworks, Please spread this question to more people.
It is better to list 5~10 tricks for others, we will accumulated more and more in future.
What are your most impressive tricks of solidworks, Please spread this question to more people.
It is better to list 5~10 tricks for others, we will accumulated more and more in future.
Andy Sanders wrote:
If you need to rename some parts or assembly files, and they're all related to each other in the same Windows directory, there's no need to open Solidworks Explorer to do this. Simply right-click on the file and pick your desired option.
It actually fires up the same dialog box that you get doing the same thing inside of Explorer.
All references are maintained doing this, as they are when you use Explorer also.
That is a great tip!! Thanks!
I wish I knew how to broaden the search this way so you can cover references that might be in other directories (like you can in Explorer).
But for me, 90% of the time all the files that are affected by the name changes are sitting in the same directory, so this works great for quick changes.
I was always in the impression that you change those options in SW File Explorer - because the tip you show above opens the same dialog box...
Ah, so what's set there works in both ways to do it? I'll have to experiment. I always reset to same directory in Explorer so I don't mess anything up accidentally.
Managing references in Solidworks without having a PDM system in place is a chore.
LARGE ASSEMBLY TIPS
This is just a few off the top of my head. Many people don't understand how to deal with large assemblies, and I've seen some good writeups with solid advice. This will probably not be new to a lot of you.
1. Top Level Assembly needs to be "stupid". ONLY mates to primary planes. If you are working on a top-level assembly on something large (20,000+ parts and assemblies), you can't very well deal with blown-up mates in a timely manner. Having sub-assemblies positioned in a manner that allows them to be mated to the three primary planes with their primary planes can save you tons of trouble. You will then never have any mates blow up in the top level and any problems can be dealt with in the smaller sub-assemblies.
2. Make lightweight configurations that suppress all small details such as hardware. Use this configuration in the top level, but the regular configuration when working on the sub-assembly itself. Also, suppress patterns and anything else such as threads that may be slowing you down.
3. Removing Detail: I do NOT recommend removing detail unless it is only removed in a lightweight configuration. For instance, many people like inserting bolts with no threads. I strongly disagree with this practice. There are several reasons. First, don't threads simply look great on a drawing? But beyond the vain, I've seen problems with not showing thread. This usually occurs when using a partially threaded fastener and somebody inserts it too far into a threaded hole or decides the nut should go on a little further than the actual threads allow. Another thing is that if the threads are there, it is easy to check the pitch and diameter so you know what to tap the mating part. Otherwise, you may have to dig around to find out exactly what thread you are dealing with. Another thing is my brother is a machinist and he is getting used to seeing threads in the CAD files sent to him and gets irritated at "lazy engineers" who don't put them in. Once a machinist sees threads in a hole, or on a shaft let's say, there's no mistaking it. Times are a-changin' and threads are here to stay. As far as removing detail, I can pretty much say that anytime detail is removed, there is a very likelihood it will come back to bite you on the backside.
4. Patterns. Pattern performance is discussed in another very good thread right now, but I don't recommend patterns in lieu of taking the time to insert each washer, bolt, nut, etc. Using mate references, this can be very fast. Patterns slow down performance, as the other thread discusses. I've found assemblies that were unbearably slow with hardware patterns that became lightening fast when I removed the patterns and directly inserted each part. Tedious, but you will save time in the long run. If you only have one or two patterns, obviously it doesn't matter, but we are talking LARGE assemblies here!
5. Good hardware. This seems obvious, but some of you are suffering with slow computers. Your company doesn't want to spend thousands of dollars on a new system. Sometimes, it takes a little prodding to get them to act. In the past, when I needed a new computer and the man wouldn't bite, I logged all the time each day I was waiting for the computer to catch up. Add it up over the period of a few weeks and extrapolate how much lost productivity you are experiencing and at what rate your services cost the company and there is a good chance you'll have a new computer soon. An SSD drive is one of the greatest improvements of late that can speed things up, so maybe only a few upgrades to your existing machine are necessary. I think SolidWorks had some sort of tool to figure out and justify a better workstation, if anybody remembers what that was.
5. References. Keep the references to a minimum. Designing in context is great, but we try to remove all in context references once we are happy with a part. For sure watch out for circular references and other cluttered modeling techniques.
6. Watch the load bar at the bottom when opening a large file. You know the one at the bottom left with the green status bar that shows you a little bit about what's going on when you are opening a file. If something seems to hang as you are opening it, for instance if you are opening Bolt X and it says Bolt X for a very long time, there may be a problem with that part. See how fast the part opens up on it's own and how fast the assembly opens when it is suppressed. There could be any number of problems.
7. Network Connection: A fast, stable network connection is a must.
8. PDM. For those that don't already know, PDM will pull the necessary files OFF the server and ONTO your local drive (preferably SSD). This will greatly improve performance when working with large assemblies and also will improve network traffic.
9. Pick the Right PDM. The wrong PDM can be a living Hell. https://forum.solidworks.com/thread/90283
10. "Large Design Review" this is a great option. When you just want to look at but not modify a very large assembly, as you are opening it there is a dialog box near the bottom that allows some options of how to open it. One option is Large Design Review. This allows the assembly to open MUCH faster and you can still move around and see everything. It allows you to do approximate measurements and you can open any parts or sub-assemblies that you may want to work on from the LDR environment. For those of you who are managing a large CAD project but are not working on the top level yourself, this is an excellent tool to be able to get in and out fairly efficiently.
11. Weldments. You probably didn't know this, but I like the weldments feature of SolidWorks. Given that your assembly lends itself to using this feature, you greatly reduce the drawing tree, mates to rebuild, etc. There can be massive performance improvements by leveraging this feature. As mentioned in an example above, one of our assemblies that I referenced saved us from using thousands of individual parts by using weldments. For every thousand parts, there are three thousand mates. The software has to evaluate all of this, and every mate is an opportunity for an exploded assembly. Weldments can GREATLY reduce the hair pulling and swearing.
12. Good Housekeeping. Keep assemblies as clean as possible. Fix errors. Make sound judgment about the assembly hierarchy. This can greatly effect performance.
13. Windows. Windows can be a huge resource hog. I have a couple of computers where Windows is hogging 10-20 percent of the CPU. Have worked with my VAR to figure it out with mixed results. Another computer I have is working flawlessly. A LINUX version of SolidWorks could be a godsend to those of us that work on large assemblies, but so far SolidWorks hasn't listened.
14. Skeleton Sketches. As discussed in this thread, there are times when skeleton sketches can help improve the stability of a large model Sometimes, instead of my #1 suggestion, mating only to planes in the top level, one may need to opt for a skeleton sketch to control the top level assembly. Especially if the top level articulates. This is not as optimum as suggestion one, but sometimes one needs to add some flexibility. The skeleton sketch controlling the top level is a far better option than mates when dealing with a large assembly. Also note that skeleton sketches and weldments go hand in hand like peanut butter and jelly.
I'm sure there's more I'm forgetting...
Yep - you forgot to re-order your list - reorder your list, unless your a last first kind of guy... To have good designs you need a good base to start with - put 14 to the top and slide everything else down - hehehe - Only then does the new #2 (Top Level Assemblies) become simple, same with the new number 5 - 6 - 12 & 13
Just adding my two cents to your 10
John Stoltzfus wrote:
Yep - you forgot to re-order your list - reorder your list, unless your a last first kind of guy... To have good designs you need a good base to start with - put 14 to the top and slide everything else down - hehehe - Only then does the new #2 (Top Level Assemblies) become simple, same with the new number 5 - 6 - 12 & 13
Just adding my two cents to your 10
Of course it depends. I got used to mating top level assemblies to only planes when building everything in spacecraft coordinates. I realized the rocket faring wasn't going anywhere (in my model that is) and that all components were positioned relative to it's origin were stationary until the satellite was deployed in orbit.
But then our sub-assembly, an articulating perimeter truss, HAD to be built on skeleton sketches because of the mate flipping that doesn't exist. We had to be able to articulate the deployable structure to ensure everything was legit. I may have never figured out a skeleton sketch until weldments was available if it weren't for the mate flipping issue.
One of the basics with using a skeleton sketch part in every sub-assembly; is getting used to having no mates for any of the sub-assemblies, unless you need multiple instances of that sub-assembly etc...
Here I open an assembly - insert the Skeleton Sketch part as the first part of the Assembly and save it as .......-000 - then I may assume that the main assembly will have (10) ten sub-assemblies, what I'll do is; while in the Main Assembly I'll do a "Save As Copy" ........-001 to .........-011 - Then I'll close the main assembly and all the files, then I re-open the Top Assembly and go Insert/Existing Part/Assembly and select the ten sub-assemblies, hover my mouse over the point of origin and drop each of those files into the Main Assembly fixed, no mating. - Now in reality you could have 10 people working on 10 different areas of the the assembly - open up the main assembly and see everything complete, if everyone follows the parameters of their assembly
The Skeleton Sketch Part, doesn't need to be void of Surfaces or Extrudes - it can be a solid model
Just the way I do things but I dislike opening a subassembly at the origin and not having a single part to be found. The same can be said for the jokers that create a part in context with the part origin at the assembly origin which is 53 feet from the actual part. I will create extra planes in the subassembly that can be mated to the top level origin and are the appropriate distance from the sub assembly origin to locate it.
There are as many opinions as there are folks alive. What is "best" for one person may not be best for another, even at the same company. The ideas exchanged on this forum are a good example of that. I like hearing the whats and whys of what other folks are doing. Sometimes it is an approach I am not too familiar with or not at all and I might give it a try. Sometimes it is something that has been there for years and I never explored it. These forums are good for exposing that.
Well said Dennis!
I'm also a strong believer in the fact that there is a lot to be learnt from mistakes also, not that one should be making them deliberately! The only way that one can assume they've discovered the 'best' way is by knowing that they've tried all other avenues including the wrong ways, the bad ways, so by this token they must have made mistakes too (not that some admit it!). So inherently we all learn from those that came before us and have taken the tried and tested routes. To those that share that wisdom I am thankful. Those that know what is often the 'best way' because of the other ways mistakes are worth listening too because they can give you an example of where error's may occur if you go the other route and thereby save you time and heartache. Whereby those who only know the 'best way' because that's what they were shown to do (no explanation), they will survive and get by with no issues but have absolutely no idea why they are following that process. So, as you've highlighted, one size doesn't fit all, and this is why sometimes "mistakes" can be an underrated little gem because it is from them that we learn what might be the 'best way' for us.
Dave.
Dave, reminds me of my old boss. Id be there feeling sick to my stomach and he used to say it's never a mistake the first time, that's a valuable learning opportunity, it's only a mistake the second time. I still feel sick in my stomach when I screw up, suppose that helps to reinforce the learning experience
Yeah, he was pretty cool. His other advice was when you make a mistake, your immediate response is often to try and fix it immediately. He said don't ever jump in. That is when you are most likely to really screw things up, leave it till tomorrow if necessary. Sometimes mistakes are like pearls an opportunity to make the job better
Sketches added to assemblies can create major circular rebuilds if not done correctly - A sketch in an assembly needs to be between the Point Of Origin and the Mates. Add a Sketch or Sketches in an empty Assembly Template and add the sketches in a folder, but make sure it is positioned here;
Now you can insert parts and let's say you really need a sketch in the assembly - you can create one using the Assembly Planes etc and then drag and drop into the Assembly Folder, now in a rebuild SW starts at the top and works down.. I did update my Skeleton Sketch pdf - see attached, also notes for this is in the third page..
If your sketch is using a part in the assembly as a reference, then you cannot drop it into the folder. But now I see that you kind of referenced that when you said, "you can create one using the Assembly Planes etc and then drag and drop into the Assembly Folder."
This is interesting.....kind of reduces the number of parts required.....and maybe this will take care of the issue where my co-worked couldn't figure out the references.
I just tried it.....I am experimenting with this type of skeleton sketch right now.....
I just started a big project and I am trying to use it on this project. I found out that if you use anything as a reference that is below your folder, then you can't add it to the folder. Kind of makes sense. I don't really plan on doing that anyway.
Hi,
1. Draw everything from the origin, and mate your parts in assemblies with respect to the origin
2. Minimize the number of features
3. While sketching keep your dimensions at a minimum and use relations instead.
4. Use equations and global variables to control dimensions
5. Use Custom Property Tab Builder to setup your properties
6. Setup your sheet formats correctly so your desired Custom Properties will be shown
7. Customize your Toolbox and hide standards and hardware you don't use
8. Make drawing templates
9. S-key and D-key
10. Customize your interface
Courtesy of Jim Wilkinson:
Use the Select All command (Ctrl+a).
If you don't pre-select anything, it will select everything in the sketch.
If you pre-select a dimension and then hit Ctrl+a, it will select all dimensions.
If you pre-select a sketch entity and then hit Ctrl+a, it will select all sketch entities
Amazing!
BTW...it works elsewhere too. In parts (outside of sketch), Select All selects all edges by default. But pre-select a face and Ctrl+a and you get all faces. And it works with selection filters. So in a part, nothing selected, turn on the face selection filter and Ctrl+A gives you all of the faces.
Documented here: 2017 SOLIDWORKS Help - Select All
Thanks,
Jim
Wow, this is true all the way back to SW 2012.
Using Design Tables to list driven values. There are some important nuances to achieving this. See Nice Trick for Design Tables to Show Driven Dimensions
I was thinking on how to memorize solidworks shortcut but so many shortcut so I decided to put it as my background,
This is really one of the best tips I've seen in a long time thanks for sharing Jaja Jojo -
I took your idea a step further and added the Command List into a sketch, using the Sketch Text feature, not a note - this sketch is in both my Part and Assembly templates, and is placed on the top of the sketches and then I suppressed it so the sketch text doesn't bog down the operating memory. With the sketch suppressed all you need to do is hover or place your mouse on the sketch in the feature tree and it will highlight..
This opens up to a brand new concept of training new people or product reminders, notes etc....
This is a good idea. Unfortunately, or fortunately depending on your point of view. it requires everyone to have the same shortcuts mapped. It would work well with one centralized setting using the settings wizard, but maybe not so for those of us who like to keep adding things.
Then again, needing to remember what each shortcut does is one thing that has kept me from using very many keyboard shortcuts rather than RMB ones.
If you need to rename some parts or assembly files, and they're all related to each other in the same Windows directory, there's no need to open Solidworks Explorer to do this. Simply right-click on the file and pick your desired option.
It actually fires up the same dialog box that you get doing the same thing inside of Explorer.
All references are maintained doing this, as they are when you use Explorer also.