Top ten Do's and Don'ts

I have seen a few lists but don't think I marked them.

For new product modeling, I submit:

1. Model with dimensions that allow easy modification of the design (sometimes easier said than done),

1. Always have "Fully Defined" sketches

2. Make use of configurations to try different sizes and features in a new design.

1. Put on most fillets and chamfers after features are made

2. When needing Draft on molded parts, make sure you avoid slivers, etc. (use Geometry Analysis for Discontinuous geometry & other things after modeling features)

1. Name Features, so they are understandable to others and yourself next month.

2. Construction of features based on Planes and Axes derived from intersections of Planes are much more stable when in new designs rather than dimensioning to surfaces that may be changed later by the addition of fillets, chamfers and such which tend to "Break" all sorts of other features.

Bo

Bo's were pretty good.

I'll add one. In in your tool,options; underthe performance tab always work with `verify on rebuild' checked.

I think other users could provide "Top 10s" for document naming/management/PDM, Toolbox use, Animator, PhotoWorks, Large Assemblies, etc.

I realize Matt Lombard and others have a lot of info they have already compiled on their sites.

Bo

1) Use model dimensions in your drawings 2) Use fully defined sketches 3) Use unique filenames for all files 4) Use the exact same name for drawings and the related part 5) Don't upgrade to a new release of SW until it's been out for at least 3 months 6) Use in-context relationships sparingly. Remove all incontext relations before releasing parts to production 7) Attend training sessions and/or user groups whenever possible

Interesting. Some of the do's so far are on my don'ts list.

do tell....

Here are a few more.

1. Always use symmetry in sketches and midplane extrusions unless there is a specific reason not to. So many times I see someone start a rectangular sketch at the corner and then later put a plane in the middle because they want to line up the part with the center of another one.

1. When investigating a drawing/model issue, open the model from the drawing view. Usually the person says "I already have the model open." and come to find out, they don't have the one open that the drawing is referencing - they have a different copy from somewhere.

2. Set up drawing title blocks with all the required boxes tied to properties. That way the users have one-stop shopping in that they can change all of them from one location and not have to go to the sheet format. This is assuming that you don't bring properties from the model.

1. Learn and use hotkeys. It's sooooooo frustrating to sit and watch someone sloooowly click icons when there are established hotkeys that everyone else is using.

2. Save, save, save........

WT

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I forgot one item that I tend to do automatically at this point.

I Save after most every few Feature creations or so. It is a bitch to create ten features and then have something hang, and have to go back and recreate 15-20 minutes of work.

Obviously this has to be balanced against the Save time, but that is minimal in all but my assembly files.

Bo

Michael reminded me, so I elaborate:

I use in context relationships to start designing some assemblies with complex mating parts, but once I get the size about right I BREAK THE RELATIONSSHIPS QUICKLY, or I am in for continual problems.

In fact, I do not understand why when you pick to eliminate external relationships, & Break All references, they don't all go away, but hey, I guess we can't ask for everything.

Bo

See comments in-line...

"Michael" wrote in news:wJ9Yf.13607$ snipped-for-privacy@twister.nyroc.rr.com:

Subject: Re: Top ten Do's and Don'ts From: "John Kreutzberger" Newsgroups: comp.cad.solidworks

--snip--

I'll add one. In in your tool,options; underthe performance tab always work with `verify on rebuild' checked.

--end snip--

DD: This is usefull with complex geometries and lots of surfaces, but not so much for prismatic solids. I might even go so far as to say that it's most useful mostly when you'll need to do offsets, shells, or exports to systems where similar operations may be performed. Otherwise, it's just a performance hit.

Subject: Re: Top ten Do's and Don'ts From: "Michael" Newsgroups: comp.cad.solidworks

1) Use model dimensions in your drawings

DD: More of a nit-pick, really. This isn't always practical. In my work, model dimensions are usually not useful on drawings.

2) Use fully defined sketches

DD: ...but the the setting to require them.

3) Use unique filenames for all files 4) Use the exact same name for drawings and the related part

DD: AFAIK, this is important only to facilitate opening the drawings from the model files. Drawng file naming conventions may be more useful than this feature.

5) Don't upgrade to a new release of SW until it's been out for at least 3 months

DD: Each new release needs to be evaluated on it's own terms. There have planty of examples of stinker service packs released 3 months after SP0.0. In most cases, users find most SPs of a release more useful than any SP from the previous release. It's necessary to evaluate new features vs. new bugs, and this will always vary with application. Granted, applying such a rule of thumb will improve your odds of not getting burned as any given release matures, but the margin of error with respect to whether a release is ready for someones application is pretty large. A lot of cost savings can be lost by waiting, just as losses can be incurred by jumping too soon.

6) Use in-context relationships sparingly. Remove all incontext relations before releasing parts to production

DD: This is another one that depends on application. Even where it does make sense to remove in-context relations, I would lock them rather than break them if at all possible. If it turns out that you need them later, they will still be available.

Hi Wayne

I've beend using my own Hot keys for quite a while, but since I have set up a new box for 2006 I'd be keen to take a look at yours. Do you have them posted somewhere?

John Layne

In assemblies mate to part and assembly sketches, part and assembly planes when possible. As opposed to part features that may be altered down the road.

Kman

Take a look around here. You will find the files related to hotkeys, macros, etc. The main file that lists all the hotkeys is SolidWorksHotKeys.xls - make sure you grab the Keypad macro files also. Let me know how it goes.

WT

"John Layne" up a new box for 2006 I'd be keen to take a look at yours. Do you have

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The heck with hotkeys, get a Sidewinder Commander (if you can find one), or a Claw or other ergonomic mulitiple input device. I bought up a couple commanders, hopefully the life of the drivers hold out.

I do the same for in context relations. I try to use the sketch geometry if possible for the exact same reason

How about this: Learn to use the established hotkeys that everyone else is using instead of coming up with your own custom arrangement. That way anyone you work with can feel comfortable on your computer and you can feel comfortable on theirs. You're all working with the same program. You can also go to other companies and comfortably use the default hotkeys.

Sure - take a look at the list. All of the hotkeys in the top portion are the ones that are standard with SW. Then to supplement those, the bottom portion has the ones we have added since they don't already exist in the software. Do you know of any existing ones that are not in the list?

WT

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Why not learn to use Windows logins so that people can use the hotkey and toolbar setup they find most efficient? A sheet metal guy probably needs different hotkeys from a weldments guy, and an ID guy will use really different stuff.

On top of that, there is variation in individual working styles. Not everybody who drives a company car uses the same seat and mirror adjustments. There is at least as much variation in how people think as there is in how they fit in a car. The current discussion is a good example.

If you are stuck in the sheet metal world or only work with solids, get out once in a while and try some surfacing, lofts, etc. Learn another area of the software. It will improve your abilities in sketching, teach you different ways of doing the same thing and help to understand how the program works.

In sheet metal, never fake what you're trying to model. Find a way to get the software to make your part.

Learn manufacturing processes so your models relate to the real world. For example, adapt your sheet metal parameters like k-factor or bend deduction to use what your shop or vendors are using.

Great suggestions on this topic. This group eliminates paying a var for unnecessary handholding services.

Thanks, Diego