Assembly standard practices

[sp1ke727]

I'm new to SolidWorks as you can probably tell in my previous posts. If this question is inappropriate, let me know.

I finished my first assembly that is work related and it looks nice, but I'm sure if someone else had to use or edit it, it would be a nightmare.

Are there any decent links that you could recommend for assembly building practices?

 

[ctopher]

sp1ke727,
Have you had training? If not, I suggest to get it.
My suggestion is to build the assy as it would in reality.
There are also videos on YouTube.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08; CATIA V5
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[mncad]

Something that would really help someone else editing your assembly in the future is organizing your mates. The mates can be added to folders. All the mates that pertain to one part can then be put into one folder that is named appropriately. Also, use subassmeblies as much as possible.

mncad

 

[MadMango]

I'll second the use of sub-assemblies and building the model as it would be built in real life. Think about how the parts are stocked too. Sub-assemblies can help to keep your top level mates below the magic 300 number, which in the past (not sure about SW09) could cause issues with some systems.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[drawoh]

sp1ke727,

If your assembly is complex, I suggest using the folders to capture related parts. At the very least, you should be able to find a part, and quickly see what fasteners are used to hold it in place.

Name your folders and component patterns intelligently. Work with your PDM people to ensure you have an intelligent file naming scheme. On my site, people go into the assembly browser and they click their way down the tree until something highlights. This is a deranged waste of time.

When you are done, change all the assembly controlled, parametric features on your parts, to features controlled within the part. There is a long list of problems here. This affects the update time of your assembly, particularly if it is large. SolidWorks updates read-only parts in RAM. This allows for randomly changing dimensions on your fabrication drawings, for which your manufacturing people will have to kill you. People should be able to re-use your parts on new assemblies, and they should be able to trust you to not change stuff without (or even with) warning.

Make sure your assembly drawing shows clear assembly instructions. If the assembly procedure looks idiotic or impossible, fix the design. For example, there are cars out there where you have to winch the engine out of the car to change the spark plugs. Documentation does not just help the end user.

JHG

 

[TheTick]

I sometimes use sketches to lay key features on an assembly. This way, key assembly dimensions are not lost if a part is changed. Key components are mated to the top level assembly sketch.

 

[SnowCrash]

For example, there are cars out there where you have to winch the engine out of the car to change the spark plugs. Documentation does not just help the end user. JHG

Nahh, just loosen the engine mounts and find a mechanically inclined jockey. But that concern may be beyond what even CAD can handle. The boss always seems to want to work on the core part which requires taking everything else apart. At least I have reduced our designs to mostly one wrench size.
One way to reduce the finished design to permanent parts is to save the assembly as a parasolids model with featureless solids, and then save the parts drawings as pdf files.

--
Hardie "Crashj" Johnson
SW 2008 SP4
Nvidia Quadro FX 1000
AMD Athalon 1.8 GHz 2 Gig RAM