End of November I had the privilege to attend the Solidworks Assembly Online Course that was offered to me by Javelin, a Trimech Company.
Yes, this “covid era” has given us and a lot of others the opportunity to attend SW courses from the other side of the world, which was not possible before! I’m very grateful for that opportunity and I try to use it to my advantage.
Training Course Contents
In case you are interested in the exact content of that course, here is the link to their training course web page.
The training was 25 hours long (5 days x 5 hours) and before the training, I received the printed version of the manual.
How I made sure I got the most out of my training
For two months prior to the training, I was putting together a list of questions that were bothering me on a daily basis but I didn’t have the time to discuss them with our VAR.
Also a day before the training I flipped through the training manual and I added some more questions on post-it notes to my manual. As we went through the manual I had my questions ready at hand.
During the training, I was also making notes about everything that I didn't know before and everything that could be useful for us in the future. These notes were mainly print screens with a few words that I keep saved in a google document for future reference.
I also did not hesitate to ask questions that were about the topics that were not specifically addressed in the manual. I shared my screen with my instructor Jamie Hill a few times, so we could test these new ideas on our customer’s projects.
My Takeaways
I decided to divide the newly acquired knowledge into a few sections based on the time one needs to “start” using them. Some ideas are really quick to implement but others could influence your company’s CAD standards so they should be tested thoroughly.
I want to point out that I will be only addressing the ideas/tips/info that I, myself, did not know about before but I believe they could also be of value to others.
- Simple tips and tools that I can start using right away
- Tools that will require some time and testing
- Tools that will require the buy-in of the whole CAD team
- Tools and techniques that we might use in the future
Interested in Large Assemblies?
We did address large assembly management a little bit during this training, but If you are looking for a more in-depth course on how to speed up “Slow” Assemblies and Drawings, I could not think of anything better than Javelin’s Large Assembly and Drawings Workshop.
We took this workshop a year ago and a big plus of the Large Assembly Workshop was that we got a recording at the end that is ours to keep! I still revisit that recording every now and then to freshen up my knowledge.
I really believe that before you go and buy a new workstation in hope that it will solve your problems with SW performance, you should first think about attending this workshop! It might save you some money and time.
Link to a quick taste video of the Large Assembly workshop
Link to Alin’s technical session from SW World (accessible with an SW ID only)
Training Days LinkedIn Posts
I also made some quick LI posts during the workshop days. Just to put everything regarding that workshop in one article, here is also the list of those:
SIMPLE TIPS AND TOOLS I CAN START USING RIGHT AWAY
MULTI-MATE FOLDERS AND LINKED DIMENSIONS
If you are doing a multi-mate you have the option to group those mates to keep them a bit more organized in the mate folder.
If you are applying a distance mate you have the ability to link the applied distance to all mates. In case you don't need that group of mates you can dissolve it afterward.
SHORTCUT TO WIDTH MATE
You don't need to select the width mate and then go and add the faces to the correct selection window. It's easier just to CTRL select the four faces to which you will apply the width mate and SW is clever enough to offer you what you need.
USE WIDTH MATE INSTEAD OF A LIMIT MATE
Limit mates are great but you need to define a dimension that might need to be corrected when you are making changes to your design.
A better approach is to use a width mate and set it "free".
DISTANCE MATE CAN BE MADE DRIVEN
Sometimes you need to position a part in your assembly but you don't know the exact distance that will be correct.
Instead of figuring the distance in advance you could apply a distance mate and turn it to "driven". Then you position it by hand and when you are satisfied with the location of your part you can then turn it back to "driving".
USE "DEFER UPDATE" WHEN REPLACING MULTIPLE COMPONENTS AT ONCE
THIS IS MY FIRST FAVOURITE
Sometimes we need to replace multiple components with a different component. If we are lucky we get green checkmarks for all replaced mates and we continue with our day. But what can we do if we get some warnings during the replacing process?
Prior to the SW training I would have replaced one component at a time and this would take me quite some time, but now I know a very nice trick:
1. Select all components that you want to replace
2. Click on Replace Components and choose the new component
3. If you then see a bunch of mates that will not be applied correctly
4. Don't worry and don't try to correct them
5. Click on "Defer Update"
6. You'll get some errors and warnings in your feature tree and that's ok
7. Select one of the problematic mates and correct it by hand
8. Now the trick: SW will recognize what you did and it will ask you if it should do the same also for the other components!
9. You click yes
10. You repeat the process for other mates that might still be red or yellow
11. You might need to force rebuild everything in the end.
This way you will only need to correct the mates of one component and not all of them which would be the case if you did not click on "Defer Update".
THE CORRECT WAY OF ADDING REFERENCE DIMENSION
If you want to add a reference dimension to a part or assembly SW first offers you the dimExpert dimension which is not best suited for this application.
Honestly, I never took a good look on the left side of the screen when adding these dimensions (I don't use them very often) so I never knew that I can choose a "Reference dimension" that does not have the tolerances attached to it.
SPECIAL ICON BESIDE THE MATES
I never noticed this icon beside the mates:
If you see this icon beside a mate it means that this mate defines the position of the component in space. If you suppress that mate you will be able to move the component.
This can be handy if you have a complex assembly with a lot of mates and you want to move a component but can't figure out what mates hold it in place...well now you know the answer.
COMPONENT PREVIEW WINDOW
Sometimes it's hard to apply mates between small parts in large assemblies or in places where you don't have much room to get a good view of the faces that you need to select. My preferred way in such cases is to use isolate but this can take some time in the case of large assemblies.
To help us out a bit, the guys at Solidworks added the Component Preview Window to our toolbelt. It helps you isolate one component in a separate window which gives you a bit more room to select the faces you need to apply the mates too.
RIGHT MOUSE CLICK ROTATES THE COMPONENT
Hah...this one is funny! I did not know that the right mouse button can be used for rotating a component in the assembly. I always used a shortcut on my keyboard to access the rotate command.
SYNCHRONIZING PATTERNED COMPONENTS TO SEED
Sometimes it happens that I accidentally change a configuration of a patterned component and this means that not all my components are exactly the same configuration. Sometimes this is what we want but sometimes this can result in an error. To prevent this from happening you can put a checkmark in the box that is nicely hidden on the bottom of the pattern feature settings.
GROUP THE SAME COMPONENTS
I like the idea of having my components grouped together sometimes. I can turn this option on or off via Tree Display options.
REMOVE WARNINGS FROM THE "DON'T SHOW AGAIN" LIST
During the training, I asked Jamie where can I define if only the assembly turns virtual or do also its parts turn virtual. He said that I should get a pop-up that asks me about this.
Well of course I must have been very wise in the past when I clicked on "don't show me again" on this particular pop-up, so I forgot that this option even existed.
Jamies advice was that every now and then it is good to check up on that "don't show me again" list.
After that, I actually cleaned up the whole list and now I am slowly building it up again but only with the pop-ups I really don't need to see all the time.
USE A MEASUREMENT SENSOR TO SEE THE LENGTH OF A 3D SKETCH
Sadly SW does not have the option to dimension the length of a path if the sketch is a 3D sketch. What you could do as an alternative is to measure the length and then apply a sensor to it. This is how I keep an eye on the length which I need to manually insert into the pipe's custom properties.
It would be also very nice if this sensor measurement could be somehow linked into a custom property. In case anyone knows how to do that, please share it with us in the comments below.
TOOLS THAT WILL REQUIRE SOME TIME AND TESTING
FLEXIBLE COMPONENTS: YES / NO?
This is quite a new feature which means it's still a bit buggy. You can check its official presentation here.
I will try to see if I can use this feature to reduce the number of configurations I need to simulate different states of a flexible component e.g. a rubber bellow or a flexible hose.
I'm wondering if making a component flexible will influence SW performance in a bad way (like it is the case with flexible assemblies). But I also believe that this feature deserves a fighting chance because I really don't like to add numerous configurations just to show a rubber bellow in any position I might need.
Below you can see how I do my rubber bellows now without the flexible component option. I have the Max and Min length configuration because I need it for the drawing. The default configuration is set to some middle position and If I wanted to show the bellow in a different length I had to make a new configuration, which is also not good for SW performance.
If anyone has tried this and has a working "flexible" version of such a rubber bellow, I'm all ears!
MAKE INDEPENDENT (WITH DRAWINGS ?)
THIS IS MY SECOND FAVOURITE
This gadget will save me some time in the future but first, we need to upgrade it a little bit!
The original "make independent" feature creates a new part based on the original part and it replaces it in your assembly. This is very useful but it would be even better if this feature would have the ability to also copy the drawing (if it exists) of the original file and save it under the new parts name.
Why do I think this is important?
A lot of times I reuse parts from previous projects. But sometimes it happens that I see that I would only need to tweak the part a little bit to make it a better fit for the new application. To do this, I need to pack-and-go the part and its drawing and save it under a new name. This process can be a bit boring and if you have a lot such parts also time-consuming.
If we had a macro that would work like "make independent" and also be able to copy the drawing and replace the referenced model accordingly it would give my work a little boost.
If you also want to use this macro you can download it here.
Thank you Artem for helping us out with this!
TOOLS THAT WILL REQUIRE THE BUY-IN OF THE WHOLE CAD TEAM
COMMENTS AND COMMENT INDICATOR
We never used comments before because they were quite easy to miss if the only indication for a comment is in the comment folder on the top of the feature tree.
But maybe this will change because now I know that I can turn on a comment indicator that shows me an icon next to the model that holds a comment!
Most probably I will use comments when I get some change requests from the customer which don't need to be done at that exact moment. Currently, I'm putting such comments on a list, but I might lose that list or even forget about it. Having the comment directly in the model (with the comment indicator turned on) might be better a better approach.
This feature will need some testing and eventually also an update of my SW templates to show the comment indicator per default.
ENVELOPE PUBLISHER
The idea of this tool is to enable you to copy a component or a device from a higher level assembly into one of its sub-assemblies as an envelope. If the device/component moves in the main assembly this will also result in an update of that component's position in the sub-assembly.
Honestly, I found it quite hard to understand how to add additional devices to the envelope group without creating duplicates and how to delete them from that group eventually. Maybe I only had this weird problem because of PDM, not quite sure yet.
I will need to test this tool a bit more to understand exactly how it works and how I can use it to my advantage and not cause other potential problems I don't know about yet.
But one thing I'm certain of. If I use this tool and when I finish with the design and I release the drawings, I will have to break the link to the main assembly. Otherwise, I might risk that someone deletes the publisher group in the main assembly which would then delete the envelopes in the sub-assembly.
If you don't design a device that is connecting two other devices which positions might still change it is probably a better idea to just use a simple insert of the components you need and set them to envelope.
CONFIGURATION TABLES
I always thought that excel based design tables were the best way of doing configurations, but according to Jamie, it is better to use the integrated version for this purpose. Actually, I never liked the Excel design tables anyway so I was happy to hear that the integrated configuration tables also enable you to put in equations in case you need them.
Below you will see an example of such a configuration table that I did for configuring the size of a pipe.
TOOLS AND TECHNIQUES THAT WE MIGHT USE IN THE FUTURE
MAGNETIC MATES AND FACILITY LAYOUT
Those could be interesting for faster creation of 3D layouts but the preparation will require some time so I'm keeping this tool as an option for the future.
If you want to know a bit more, here is a nice short article.
TOP-DOWN MODELING
We do use some top-down modeling techniques but once the design is finished all the references need to be broken and clearly defined.
Actually, I'm not a big fan of "over-advanced" top-down modeling techniques because they may differ from user to user and this can cause problems in a larger team if changes need to be made. I rather have it clean and simple once the design is released.
I wish to learn more about this topic in the future as it might come in handy during the concept phase.
MATE CONTROLLER
This tool might also come in handy in the future because it looks like a very nice alternative to the motion study. The problem with the motion study that I have is that it is not very intuitive and I get easily lost in all the options.
Besides this, the Mate Controller also enables you to make an animation!
SMART COMPONENTS
Smart components might be handy to those who frequently use components that always need the exact same feature (usually holes) to be made on the part to which they are mounted.
Probably this is most handy for users who work a lot with electronic components.
For our work now I don't see much use in smart components but I kept it on the list as a reference for you.
TREEHOUSE
Although we use this tool only if we need to visualize a complex assembly structure it can be used for much more.
Thinking now as I write:
For us, it would be especially useful if Treehouse could generate an interactive file (maybe a PDF) that would give someone without SW installed the ability to dig through the structure as it is possible to do in Treehouse. The reason for this is that if I want to share the structure of a large assembly with someone else, I need to make a PDF. Such PDF is usually not very nice for printing and also not for scrolling left and right.
At least what we would need is to have a PDF that has the ability to search for a specific item by hitting "CTRL+F" and typing in the item number! The pdf version that I generate with an ordinary PDF Printer does not have this ability. If anyone knows how to make this PDF searchable, please let me know.
COMMENTS WELCOME!
In case you have any questions or ideas on how to use the presented tools even more efficiently, please do not hesitate to write in the comments or to contact me directly.
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