Equations and part configurations 2

[mkmech]

I have an assembly which contains several different configurations of a part. I want to create an equation that will contain dimensions specific to a certain configuration. But doesn't look I can do that.

Let me clarify with a simple example: let's say the part is a cylindrical rod. This part has multiple configurations and the configurations differ in respect to the length of the rod. Now I insert several instances of this rod into an assembly. Some of the instances are different configurations (i.e. different lengths). Now I want to create an equation such that the equation will only affect a specific instance (configuration). But when I select that dimension (length in this case) to add to the equation, it looks like that the equation doesn't differentiate between the configurations and changes the length of all the instances (configurations).

Please suggest if there is a way to do this.
Thanks to all the readers.

 

[TheTick]

Equations can be suppressed on a configuration-specific basis. I [highlight]highly[/highlight] recommend that any config-specific equations be controlled with a design table. They can get twitchy, otherwise.

Also, always good advice w.r.t. equations: <faq559-590>

 

[TheTick]

Oops, didn't read carefully enough the first time...

Not so sure how to get around your specific problem.

 

[macPT]

Try to create a custom property lets say change_length. This will have value 0 for non changing and 1 for changing, for each instance.

The amount, in the equation, to change the length will be multiplied by change_length. This way only the selected instances will change (those with change_length=1).

Regards

 

[mkmech]

Thanks macPT and TheTick. I appreciate your comments.

 

[TheTick]

I think I have a solution (provided I understand your problem correctly).

Problem:
You wish to control a configuration-specific dimension in one component's configuration but not the rest of that component's configurations.

Solution:
[ul][li]In the part file, control the dimension by a configuratioon-specific equation, linking its value to a dimension in a control sketch.[/li]
[li]Use equation in assembly to govern the dimension in the component's control sketch.[/li][/ul]

"An object at rest can not be stopped."

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[mkmech]

TheTick,

Can you elaborate on the solution? I didn't quite get it.
1) What is a control sketch and how do I create it? is it different from the part sketch?
2) How do I create config-specific equation in an assembly? Also, with reference to your previous comment, how do I suppress a given equation so that it doesn't apply to a particular part configuration in an assembly?

macPT
There is one problem with your solution - the equation will contain the final length of the part and not the change in the length. For example,

length@Part1.prt = Diameter@Part2.prt + Thickness@Part3.prt

If I use your solution, my equation will look like:

length@Part1 = change_length@Part1 * (Dia@Part2 + Thickness@Part3)

Now if change_length=0, then length of Part1 will become zero which is not what I want.

Do you have any suggestions? I would love to have both yours and TheTick's solutions.

Thanks to both of you.

 

[macPT]

You're right mkmech.
My idea only works on something like:

new length = initial length + increment * control flag

For the moment two ideas :

1- controling the dimension with an IIF statment.

new length = IIF(control flag LIKE 1, equation if true, equation if false)

2- controling with DT, on which the length column is controled by an EXCEL IF function

Regards

 

[CMcF]

I have just modeld a cylinder. In one config the length is 2 times the diameter, and in another 3 times. In the part sketch I dimensioned the length twice. 1 dimesion driving and the other driven, and applied the equation. I then changed config, edited the sketch and swapped round which length dimension was driving and which was driven (cofig specific using dimension properites), and applied a new equation to the now driving length dimension.

It seems to work even without config specific suppressing equations.
It helps to rename or lable the dimensions.

Hope this helps.

 

[mkmech]

Hello all

I am restarting this thread as I was not clear about some of the solutions proposed. I will appreciate any clarifications or fresh ideas.

CMcF:: If you model the cylinder by extruding a circle, you can't dimension length because length was created by extruding and not through a sketch.

TheTick: I quite don't understand the concept of control sketch. Can you elaborate?

Even though several solutions were presented, I am not sure if these would work if the part was complex and had several dimensions and several configs. Also, macPT proposed "controling with DT, on which the length column is controled by an EXCEL IF function". macPT, do you mean I should create a DT in the part file or assembly file?

Any more suggestions?

Thanks to all.

 

[CMcF]

mkmech,
Oh yes you can! (sorry , panto season).
Create your cylinder, by extruding a circle. Once you have the cylinder, double click one of its' faces. Voila the dimesion for the length apears before your eyes!

This also works for chamfers, fillets, the number of instances and pitch in a pattern.

I would normally select the elusive dimension, RMB properties and rename it to something useful.

Another way to find elusive dimensions is to create 2 cofigs of a part. Insert a design table with the option auto-create selected. All the config specific dims will be inserted into the table.

Regards,

Colin



Regards,

Colin.

 

[TheTick]

A control sketch or skeleton sketch is a sketch used to create curves and dimensions for control purposes only. No solid features are made from the sketch. Solid features that need to use control sketch geometry do so in a separate sketch and copy the sontrol sketch curves using convert entities.

This makes for a more robust model that can accept major changes more readily.

We make lots of hinge assemblies. I uually create a control sketch for the whole assembly at the top level and copy parts of that sketch to control sketches in each of the components.

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