Link values of different components in an assembly 2

[adymech1]

I am trying to link two dimensions that are in 2 different components in an assembly. I tried linking them but it doesn't work. Does linking values only works if I link 2 or more values in the same sketch?

 

[CorBlimeyLimey]

"Link" does not work between different parts in an assy.
You will have to use equations instead.

from (the City of) Barrie, Ontario.

What happens if you get scared half to death twice?

 

[SBaugh]

They have to be in the same part. Equations might get you there, but from my understanding and the way it has always b een in the past. You can't link dimensions fomr one part to another, via an Equation or DT. This is where In-context relationships play a role in SW. Dimensions are no longer the control agent in the part. you can in-context a sketch or a feature using planes in the assembly. - see faq559-871.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

If you are in the SW Forum Check out the FAQ section

To make the Best of Eng-Tips Forums FAQ731-376

 

[adymech1]

Thanks a lot to both of you!

 

[CorBlimeyLimey]

You can't link dimensions fomr one part to another, via an Equation or DT.

from (the City of) Barrie, Ontario.

What happens if you get scared half to death twice?

 

[CorBlimeyLimey]

Ooops ... wrong button

Sorry Scott, I have to disagree ... Equations can & (as far as I know) always have been able to use a dimension of one part to control a dimension of another part in an assy.

Try it and see with a simple Width@... = Length@...

from (the City of) Barrie, Ontario.

What happens if you get scared half to death twice?

 

[SBaugh]

Your right Equations do work. I haven't used Equations much when making my assemblies. I used DT and In-contexted relationships, but I was also doing a lot of Automation and that required in-contexted relationships.

I'm pretty sure there was a time when you couldn't control a part like that, but then again I might be wrong.

I was always told this for years. But things change and sometimes it's hard to keep up. Thanks for pointing that out CBL.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

If you are in the SW Forum Check out the FAQ section

To make the Best of Eng-Tips Forums FAQ731-376

 

[neilc78]

I just looked this up as I am trying something similar. It appears to me that the use of equations between parts in assemblies does not work if one of the driving dimensions is controlled by configurations.

For a simple example.

I have two parts in an assembly called 'Box' and 'cylinder'. The length of the box is set to equal the length of the cylinder by an equation. However, If I then create a number of configurations of the cylinder (controlling its length) and then change the configuration of the cylinder used in the assembly, the square will not update (or at least I can't get it to) - Has anyone come across this before? Anyway around it?

 

[SBaugh]

No you can't control a Part's Dimension from either a DT or an Equation from the assembly level or from another part level. You must In-context it in the assembly. See help on In-contexting.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[neilc78]

I have come up with a solution/Work Around which suits my application. Again I will use a simple analogy.

I have a cylinder with wall thickness 'T' and I want this to stay equal to the side of cube 's'. The cube has numerous configurations. Lets say I need to control this by an equation in the assembly. Here is what I did. In assembly mode select sketch and select a face of the cube as the sketch plane. Select an edge of the cube and then convert entities. Now also dimension this line. You will get the overdefined warning. Right click on the dimension and select 'Driven'. That will remove the error.I will call this dimension 'd' from now on.
Now you have a dimension inside the assembly that will change as the cube component configuration changes, as will the driven dimension. You can now use dimension 'd' to define dimension 'T' (i.e. set T = d). The only draw back is that you will end up with a load of 'dumb' sketches in your assembly. The other problem is that you cannot do this for things like quantities of features in patterns. I wouldn't recommend as a design methodology but I find it neccessary in one or two eqn's within my assembly.