which plane? 1

[koyote5]

when creating a new part in solid works it asks you to choose a plane in the assembly onto which to sketch. it is better to sketch parts on the parts planes or the assembly planes and why? what if i am doing a top down assembly and decide to update the assmebly drawings to which the part drawing are associated (on edge for example)? or even decide to use the parts in a differnent assembly?

 

[CorBlimeyLimey]

This very much a personal preference ... I don't believe there is a definitive right or wrong way ... just what works best for you, the product & your company. Some methods I have read about or used:-

1) Create everything in Top Down mode & leave the parts fully incontext with the assy. This makes full use of existing geometry to create parts & makes changes easy ... update the assy (or the parts) & the parts (or the assy) will automatically be updated ... trouble is, unless you are fully knowledgeable about how the assy & parts are parametrically linked, you may not know which parts get changed .

2) Create everything in Top Down mode & then break (or even delete & redimension) all the parts in-context references when saving for production. During the pre-production release the same Pros & Cons as above apply. After production release, any changes have to be made on a per part (& corresponding assy feature) basis which can create more work, but will give greater part & assy feature control.

3) Create everything in Bottom Up mode & then create the assy by inserting the "standalone" parts into it. This does not utilise existing geometry & in effect, is not much more efficient than using a 2D product.

One problem (for me anyway) with the Top Down approach, is that the created parts origin will not be placed at a "logical" position in the part. It could be totally outside of the parts geometry, which does not easily allow for using the parts main reference planes when mating into another assy.

Now, before creating a new assy, I will create & save, a set of named "dummy" part models that I think I will need ... in other words the models have no geometry ... just a name & whatever custom properties I decide to assign. This way, when I insert it into the assy, I am forced to use the main reference planes (or axes created from them) for mating & the parts origin will always be where I decide it should be. The parts geometry can then be created, in-context or not, to whatever geometry exists in the assy. As for the in-context refs, most times I leave them intact, but sometimes I will break them if I know that part will be used in other unrelated product assemblies.

There are bound to be other people who employ different methods which work equally well for them.


Making the best use of this Forum. faq559-716
How to get answers to your SW questions. faq559-1091
Helpful SW websites every user should be aware of. faq559-520

 

[aamoroso]

I only use Top Down design when I am working on "One of a Kind" designs that I am working with little outside input or guidance to the end product.

If someone is driving my design with sketchs and drawings of parts, then I avoid it, same when someone is micro managing a project.

I also avoid Top Down when I am working a project with lots of configurations and alternative designs.

I also avoid Top Down when components created for the assembly are likely to be used in other places.

Fill what's empty. Empty what's full. And scratch where it itches.

 

[ctopher]

The more we use CosmosWorks, the less we do top down design. Because some features in parts have to be removed or suppressed to work. I create about 95% of our designs bottom-up. Every part has the origin and planes in the correct placement and each can be exported/read to CAM or the cutomer easly.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP2.0 / PDMWorks 05
ctopher's home site
FAQ371-376
FAQ559-1100
FAQ559-1091
FAQ559-716