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Assemblies people! Not assemblies of people, which can have you going through more gallons of fake blood than a remake of the Re-animator, but assemblies of inanimate chunks of 3D data.
You can make really, grossly huge assemblies but there’s a point where people start whispering about you behind your back. Instead of spending your morning talking gossip with the office manager while your models load, split them suckers up and do a little dance that will also have people talking behind your back.
Four Reason to Hack up Assemblies
There are 4 reasons why you would want to start choppin’ up a fine mass of plastic, steel and screws and it’s all about small. Small stuff that makes a big difference. Now isn’t that clever?
- smaller file sizes
- smaller BOMs (Bill of Materials)
- smaller drawings
- smaller FeatureManager mess
Building these four ideas into your methodology alone can help keep your assemblies in a more manageable state. Dwell upon them, stare at the ceiling repeating them in a low monotonous voice and then also use these four techniques to split them up.
1. Combine parts that don’t attach together
Can you see the possibilities opening up already? A group of connected parts that attach to another group of connected parts is typically how we think of sub-assemblies.
Thats a fine approach to creating assemblies, but remember as you read the rest that any part or assembly can go into another assembly.
2. Create yourself some sub-assemblies
Phenomenal concept, hem? Well, you’ve got everything in the assembly to the point it’s overwhelming you and your computer. Considering what to put into sub-assemblies is the first step. Here’s four possible solutions.
- Parts that are manufactured in the same place
- Parts that are or could be put into kits
- Raw material parts only
- Hardware only
Once you’ve thought that over, you can go to your FeatureManager, find the items you want to combine, hold the Ctrl button while selecting them, then right-click and select Form New Sub-Assembly.
3. Dragin-n-Dropin-n-Dragin
Yes, so obvious, using the mouse to move items into and out of assemblies. Simple, yes, but don’t be afraid to do it. After you’ve formed some sub-assemblies and created some drawing views, you may decide something would have been better off in another location.
To get an item out of a sub-assembly and into the top assembly, drag it to the very top line in your FeatureManager. If you already know where you want to put it, drag it straight into the other sub-assembly. It’s something pretty basic, but not all that comfortable to do until you’re use to it.
4. Optimizing your drawing
You most likely have a standard for your drawing layouts. It would be great if everything could fit on one sheet, but sometimes models need a little bit more detail. Here’s a few questions I ask when harping on making drawings more simple.
- Can those 4 drawing views be reduced to one exploded isometric view?
- Is all of the detail needed or can I show some sub-assemblies as reference?
- If it’s not providing any value is it needed?
After checking a drawing and asking this, I’ll see what I can eliminate and how I can combine parts into -subassemblies to get a better looking drawing.
A note on top-down design
SolidWorks 2007 and 2008 are pretty good at keeping relations when moving parts around. SolidWorks2008 gets rid of the annoying “This part has features defined in the context of another assembly…” warning. So, if you work in large context driven assemblies moving to SolidWorks 2008 can save you a lot of pain of dealing with contextual relations. Rockin’.
Are there better ways to create a drawing or assembly or part? I think it’s something we need to ask every time we start something new.
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This is a solid post that works for me Josh… (no pun intended). Your 4 ’small’ reasons to hack up assemblies just make sense. However, I struggle sometimes knowing how far to go. I often run into assemblies that have 300 - 1000 parts but only go 3 sub-assembly levels deep. That sometimes makes for several hundred top level mates (sure to slow it down correct?). But I hate breaking these up any more and keep trying to maintain consistency in part numbers and manufacturing/assembly process. But in my experience I believe I have other factors that affect load times and performance (no specific order).
1. Opening/saving files over company network
2. Many sheet metal parts
3. Part patterns
4. Top level mates
5. Assembly cuts
6. External references
Agree/disagree with anything?
Hey Ivan! Thanks! Everything you mention can slow indeed slow assemblies down. I’ve done another post on improving Large Assemblies performance.
When you get assemblies that large, you’ll want to suppress some of those complicated feature. I’ve gone as far as suppressing all my mates and fixing everything.
I would make sure drawings are split up so that different production steps are kept separate. I suggest keeping construction drawings separate from build/assembly drawing. when trying to do both on the same drawing, it can turn into a very large and unclear mess. This get tricky because everyone has there methodologies driven by different reasons. If you can show how drawings can be improved and get productions help it makes changing assembly methods easier.
I would try to “flatten” out your structure as much as possible. I try to stick to two levels deep. More is fine, I just try to keep it as shallow as possible.
Hope this provides some further clarity for you. Assemblies can be a real beast but it fun to see how other come up with ways to handle them.
I pull in IGES data for vehicle layout studies all the time. I can’t put into words how much I hate waiting for large assemblies.
hi Ivan
You can get rid of a lot of the items you listed slowing down your assemblies. Part patterns can be Dissolved by Right clicking on the pattern feature once you know how many you need or could be done in a sub assembly instead. Top level mates can be reduced by first mating components into place then fixing them. In 2007 and 2008 the mates are suppressed automatically (so you can go back to them)but wont be rebuilt everytime.
Assembly cuts could be done on the actual parts in another configuration of the part and External References could be locked while you are working on the assembly (RMB then List External and Lock, like breaking but you can get them back).
To stop working over the network, speak to your reseller about PDMWorks Workgroup or Enterprise. The file open time will be the same but when you hit save it will save onto your local drive so that will be much quicker. Its also automatic revision control so not a bad thing.
Ivan,
Working local versus working over the network should give you the biggest performance boost of all. You should check out PDMWorks Workgroup. Since it is packaged with SolidWorks Office Professional, you may already have it!
Great post Josh!
Best Regards,
Ricky Jordan
http://www.rickyjordan.com
Thanks for the ideas guys. I find myself fighting with things like assembly features and external references. It’s a tough call, because it greatly speeds up design, does all this cool stuff and updates with design changes, while at the same time takes a hit on performance. And I know everyone’s situation is different. I really believe my biggest bottleneck is the network.
So… we do have PDMWorks. I’ve never used it and therefore am not confident enough to dive in. We make a lot of one-time custom projects, so I guess all the control that PDMWorks gives you seems kinda stifling to me. But I love the concept behind it and I’m sure we could customized it to suit our needs. Does anyone have some handy info on implementing it?
PDMW Workgroup is dead easy to set up straight out of the box. You basically install the PDM service on a server and it sets up a Vault where all the files go to. Clear firewall ports 20000, 30000 and 40000 if there is one between server and clients. If you have Office Pro you will already have the client installed. Fire up sw and add in PDMW Workgroup. If you dont have it you will need to modify your SW Explorer install to include the PDMW add in and the VaultAdmin tool etc. Then, all your settings are in the VaultAdmin tool. Without the training (only 2 day course, 1 day admin, 1 day user training) i would leave the Lifecycle management and just choose your revision scheme and general settings to suit. Hope that helps!