How Many Constraints are needed to Fully Define a Sketch 4

[Scott4tg]

I am using SW2007 and am working on an aluminum extrusion sketch that is a library feature to be inserted into a weldment later. The sketch has three profiles along the base that are identical. I am trying to get the sketch fully defined without have a gadgillion dimensions on the sketch. Is there a simple rule of thumb to follow when defining a sketch??

Any help would be appreciated.

Thanks in advance.

Scott

 

[ctopher]

Use the proper dimensioning to define the feature until it turns black.
Don't throw dims everywhere until it is defined, proper dims will define it with the least amount of dims. The machinist can also use these dims.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 09-17-07)

 

[JMirisola]

You could always just RMB and select 'Fully define sketch'...

Jeff Mirisola, CSWP

http://designsmarter.typepad.com/jeffs_blog

Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

 

[CorBlimeyLimey]

You could also select all geometry and use the Fix option.

NOTE: Although the Fix and Fully Define Sketch options will define the sketch (and turn it black) they will not capture any Design Intent ... or even give suitable dimensions for machining.

 

[ctopher]

The Design Intent per CBL's note is what I was also trying to say.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 09-17-07)

 

[Eltron]

I prefer to set all of the pertinent relations first, then dimension later. This captures the design intent with the relations, then specifies sizes second. It helps to keep the number of dimensions down. You have to be careful with the Fully Define Sketch tool. Sometimes if Fully Overdefines the Sketch...

Dan

http://www.eltronresearch.com

 

[Theophilus]

I use lots of Equal relations (and other types) to minimize clutter and simplify future edits (always editing everything I do)--so a few dimensions can control a lot of geometry.



Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe transcends reason.

 

[JMirisola]

Eltron and CBL bring up very good points. To fully define your sketch, create relationships between the profile to keep them identical. If their spacing is equidistant, and will remain that way, you can create two of the instances using a linear sketch pattern.
Without knowing your design intent, as well as what the part actually looks like, it's not easy to give you an exact answer as to what you should/can do.

Jeff Mirisola, CSWP

http://designsmarter.typepad.com/jeffs_blog

Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

 

[meintsi]

When designing library features for use later, try to stay away fron the vertical and horizontal constraints and favor the parallel and perpendicular.

When inserting on a plane perpendicular to the plane that the library feature was created on, many errors arise because it cant solve the horizontal if its inserted vertically. (Hope that made sense.)


Remember...
[navy]"If you don't use your head,[/navy]
[navy]your going to have to use your feet."[/navy]

 

[TheTick]

The sketch has three profiles along the base that are identical.

Sounds like you could constrain one profile and then pattern it.

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help