Suppress Constraints/Dimensions to obtain diff configs

[CADone]

Hi,
In a simple SW2007 part, rectangular sheet metal plate with origin in the center. I have a cut extrude feature (Say a rectangular hole) that needs to have different location with respect to origin for 2 different configs.
I need to do this manupulating the same cut feature. So in the sketch, I will have Dim X and Dim Y for this feature.

My reqd configs :
Config 1 : X = 2 and Y =2 ( I am able to achive this)
Config 2 : X = 0 and Y = 0 (I cant achive this; The cut is conciding is on the origin)

For config 2 ; Is there a way that I can supress the positioning dims and use a coincident constraint ?

Thanks
BMR

 

[Timelord]

bmr,

Solidworks doesn't like dimensions that are zero. Draw and dimension a construction line away from the origin and then dimension your feature to it so it evaluates to a positive value for both cases.

Timelord

 

[CorBlimeyLimey]

Yes you can suppress the dimension mate and add a coincidence mate for the other config.

 

[Timelord]

CorBlimeyLimey,

How do you supress a dimension in a sketch? Is this something that is relatively new, (I am working with SW2005) I don't see how to supress a dimension in a sketch. I can see a check box for suppressed in the relations property manager, but I cannot get it to work the way bmr needs it to. If I check the supressed box and add the coincident relation for the config that requires it, when I go back to the other config, the dimension has reevaluated to zero and it cannot be changed. Strange behavior for sure.

Timelord

 

[CADone]

CBL,

I am have same problem. Can we supress sketch relations (coincident)
Please throw some light.

BMR

 

[Timelord]

bmr,

I got the suppression thing suggested by CorBlimeyLimey to work, but it reverses (flips to the other side of the origin) one of the dimensions every time. If you do it the way I first suggested (dimension it to a point off the origin such that the dimensions are always non zero), it works correctly every time.

CorBlimeyLimey - Thanks for the post, I learned something new today. It just doesn't work your way when the dimension goes to zero.

Timelord

 

[CorBlimeyLimey]

Timelord ... glad to hear you learned something new, but I have to admit that I was totally off with my answer. For some reason I had it in my mind that assy mates and not feature constraints were being questioned.

 

[CorBlimeyLimey]

OK trying to redeem myself here;

Instead of using a dimension to control the sketch line, offset a new plane from the main ref plane and constrain the sketch line to it. The offset dimension of a plane can be zero ... at least it can be in SW07 ... and it does not flip sides when the offset dimension is changed.

 

[J-C]

Instead of using a dimension to control the sketch line, offset a new plane from the main ref plane and constrain the sketch line to it. The offset dimension of a plane can be zero ... at least it can be in SW07 ... and it does not flip sides when the offset dimension is changed.

When did they change that.......wow, that will be handy.

Jason

SolidWorks 2007 SP4.0 on WinXP SP2