Do's & Dont's from the Real World 5

[TateJ]

I just got a part-time evening gig - teaching SolidWorks at my local technical college. And I'm dang excited about it! I plan to share this site with my students as a valuable resource. My first class is August 23... I'd like to start a list of good & bad practices to incorporate into the class. I want to be able to share what other users are doing & not just my experience.

For example:
-> I have never used an ENVELOPE to select parts in an assembly. I use it as a refernce part for equipment layout & design. Does anybody find it useful as a selection tool?



SolidWorks 2005 SP03.0 / Windows 2000 Professional

 

[TheTick]

tidbits...

•Never use a dimension when a constraint will do.

•Merging centerpoints of two sketched arcs makes them permanently concentric.

•90 degrees is not the same as perpendicular unless the measure window actually says "perpendicular".

 

[TheTick]

I'm a big fan of layout or control line sketches. Complex parts endure changes better if they are based off one or two layout sketches that aren't directly assimilated by another feature. From there, make liberal use of "convert entities".

 

[macduff]

halfmark,
You get a star! Eggcellent point.....!

Macduff
Colin Fitzpatrick
Sr. Mechanical Designer
macduff's SW page
Inhouse System
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SW2005 Office SP 3.1
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NIVIDA Quadro4 750 XGL

 

[CorBlimeyLimey]

Congratulations & Good Luck.

My suggestions:-

Most important of all ... teach them how to use the Help files.

Give them a thorough understanding of what is in the Tools > Options{/b] section & how the options therein affect SW.

Show them how to customize the toolbars & add in the "missing", but often used, icons.

I've lost track of how many questions could have been easily answered by a quick check of the above three items.



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[CorBlimeyLimey]

I've even seen the initial sketch is the full part, and then they convert entities off that. The reason they said was to edit everything at once....these type of files can never handle change.

These are known as Control (or Layout or Skeleton or Reference) Sketches &, like TheTick, I use them very often & have found them to actually improve the stability of complex parts & assys. They also do help greatly when modifying the part/assy, as all (or most) of the features can be manipulated from one location.
With the inclusion of the Sketch Blocks abilities in SW06, I think you will see a strong shift toward this method.
FWIW, I highly recommend it.


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[ejc]

Incontext parts!!!
I have had many a nightmare when trying to modify these types of parts. I won't realize that the previous owner created the model in context of something else. When I try to modify, the whole part implodes. Usually it's easier to just redraw.

Also, referencing the parts to standard planes. Many a rebuild error was due to a little noticed dimension referencing the sketch in space.

-ejc

 

[MadMango]

In-context parts are great for design and development work, but I have found that in-context relations should be removed for standard production work.

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
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[TateJ]

That follows the KISS rule... Keep It Simple Stupid for the next guy who picks up the model. When I was still a little green... I got carried away with putting all the intelligence I could squeeze into a part or assembly. Then - 6 months later - I confused myself trying to edit my own model! I have since then - backed off a good bit. I still use the power of the program when I need it - but I remember that I'm usually the idiot I need to idiot-proof models for.

These are good tips - keep 'em coming...

I'll add one: Never use more MATE than necessary. you can use 3 coincident mates on 3 faces to assemble 2 cubes if you want to & you'll get away with it 99% of the time. But one day a very complex assembly will krap-out & after spending the time - you'll figure this one out too.

SolidWorks 2005 SP03.0 / Windows 2000 Professional

 

[smcadman]

Whenever creating parts, such as extruded items and sheetmetal, use "Mid Plane" as the base for extruding. This can make mating easier in an assembly.

Whenever creating assemblies, if possible, make the "fixed" part centered on all 3 planes; this makes mating easier because several sub-assemblies can be constrained on center planes.

If you have a pattern of holes, create 1 hole and pattern it instead of creating all holes in 1 sketch. 1 line of thinking says that your tree is smaller with all holes in 1 sketch; BUT if you create 1 hole and pattern it, you can make a derived pattern at the assembly level and insert several bolts/screws in 1 shot.

Flores

 

[ShaggyPE]

I agree whole heartedly with MadMango's post about the usefullness of in-context parts and the necessity to remove those links before the part moves into production.

Concerning smcadman's post about hole patterns, I prefer to use the hole-wizard. Within the assembly, patterning the hardware will occur as well.

 

[drawoh]

How about keeping origins, planes and sketches turned off unless you are using them.

I just hate it when I insert someone else's assembly into my design and find myself staring at a cloud of origin points. The usefulness of this feature is significantly reduced.

Model parts in approximately the colour they will appear in the final assembly. If you want to differentiate between two parts of the same colour, wiggle the colours just a little. It makes it so much easier to visualize the final CAD model.

JHG

 

[MadMango]

Always "ground" the first inserted model of an Assy to the Assy's orgin.

Always "ground" the first sketch of a part feature to the Part's origin.

ground= constrain

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[ctopher]

I always create parts with the origin at the center on the mounting surface. Parts that sit horizontal or are turned on a lathe, are modeled with the origin at the center. This helps with alignment in assy's, importing to CAM, and showing CG.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
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[chancey]

Fully define all assemblies. I've seen assemblies blow apart because of something simple like a round part rotating. This will also make it easier to troubleshoot your assemblies when faced with mate errors.

 

[TheTick]

more generic advice...

Use the modelling approach that best suits your design or product.

I see a lot of different and conflicting opinions. Most are valid in their context.

I do a lot of consumer product design that has different demands than designing machine components. I need layout sketches to define complex geometry which needs to be carried through to multiple features. Usually this also requires no mates, everything (except fasteners) modelled with a common origin.

Designing machine tools or simple components doesn't require this kind of approach. Especially true for parts that are used multiple times or in multiple contexts.

 

[TheTick]

more idle preaching from Tick

Don't forget, it's all about the design.

If you need to add sketches to define or control a datum plane, do it.

If you need to define two surfaces to get their intersection, do it (and then use "delete bodies" to clean up).

If you need to draw two sketches to combine in a third, do it.

If you find yourself changing the design for the sake of your CAD program, it's time to get help.

 

[TDFINC]

Name or describe features in the feature manager tree. This will help six months from now when you need to go back and edit that part. It can help you figure out how you created that goofy feature in the first place.

Uh? What does " Tools > Options{/b] section " mean ?

 

[chancey]

Nameing features looks nice but all you really have to do is pick the model feature and it highlights in the feature manager tree. Although, I do name planes that I create.

 

[MadMango]

TDFINC, Tools>Options is directing a person to use the menues in SW. Click "Tools" in the menu bar first, then click the next available menu selection, "Options".

[green]"I think there is a world market for maybe five computers."[/green]
Thomas Watson, chairman of IBM, 1943.
Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[CorBlimeyLimey]

The "Tools > Options{/b]" was a typo. It should have been [ignore]Tools > Options[/ignore] so that it displayed emboldened, as Tools > Options


Making the best use of this Forum. faq559-716
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