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For what type of dimensions should I set the parameters?

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For what type of dimensions should I set the parameters?

First I'd like to apologise if this question has been already asked by someone else but I didn't find similar. 
I've got a question about using parameters for dimensions. I understand meaning of parameters and also know how to use it. I know I should set parameters for some informations which can be useful in Drawing (e.g. inside drawing table) later (like material parameters, part/asm name, etc.) and I heard that I also should set parameters for some type of dimensions. The problem is I cannot find out in which situations should I do it. The only tip/answer I found is that I should set parameters for dimensions that can be changed in time. But... all dimensions can be changed while working on project actually. So, could you please explain me when to set parameters for dimensions?
Also if you have some another informations about parameters and its using I'd be grateful for giving it.

Thank you very much in advance! 

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Re: For what type of dimensions should I set the parameters?

He is making the part dimensions so they are driven by a parameter. If you know your part is going to change and you MUST keep certain relationships from one dimension to the others, you can do that using parameters and relations. It's based on your design intent and if you feel you must control that aspect of your part instead of leaving it up to the user to remember to make those changes. You can make your part as "smart" as you wish.

Remember, when another user opens your part and needs to make changes, if you make it so complicated that the user can not figure out or doesn't want to take the time to figure out what you have done, they will likely simply delete your relations/parameters.

It all depends on the type of parts you are doing. If you do springs and gears and other parts that are driven by formulas, you should master the use of relations/parameters.

I'm sure there are other opinions on this but I personally only rarely use relations/parameters.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

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7 REPLIES 7
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Re: For what type of dimensions should I set the parameters?

On your average parts/assemblies, I would say that it is unusual to make a parameter to control a dimension.

If you are trying to make families of part or all your parts use relations to control shape/size, it may make sense to use parameters or you are trying to drive your parts program-matically with some sort of automation

What kind of parts/assemblies are you planning on designing? 

 


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)
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Re: For what type of dimensions should I set the parameters?

Thank you for your answer! I ask generally. I've never set parameters for dimensions before however I read and heard I should do it - that's why I'm asking. Furthermore some of tutorials contain this practice (assigning parameters for dimmensions). I'll give you on of them where lecturer explains using parameters by assigning dimensions to them:
https://www.youtube.com/watch?v=BSMOM7W6M-U

The problem is that, as you said, it's unusual to control simple dimensions by parameters so I'd like to know in which, let's say, dimension cases we should use parameters. Is there any rule or good practice about using parameters in that cases?

This video demonstrates how to use parameters and relations in creo parametric. Just one click and the thickness will be changed in all the places where thic...
Highlighted

Re: For what type of dimensions should I set the parameters?

He is making the part dimensions so they are driven by a parameter. If you know your part is going to change and you MUST keep certain relationships from one dimension to the others, you can do that using parameters and relations. It's based on your design intent and if you feel you must control that aspect of your part instead of leaving it up to the user to remember to make those changes. You can make your part as "smart" as you wish.

Remember, when another user opens your part and needs to make changes, if you make it so complicated that the user can not figure out or doesn't want to take the time to figure out what you have done, they will likely simply delete your relations/parameters.

It all depends on the type of parts you are doing. If you do springs and gears and other parts that are driven by formulas, you should master the use of relations/parameters.

I'm sure there are other opinions on this but I personally only rarely use relations/parameters.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

View solution in original post

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Re: For what type of dimensions should I set the parameters?

No hard and fast rules for doing this.

He did it to drive multiple dimensions for his part to be controlled to the same thickness.

Could have done it with a simple relation of d24 = d23 instead of setting each to the T parameter.

 

As Stephen said, it needs to be understandable so others can also follow your logic.

 

I do a lot of modeling where I use relations and renamed constraint names. If the OD of a cylinder is d2, I will rename it to OD and then use OD in my relations.

 

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Re: For what type of dimensions should I set the parameters?

Thank you both very much for explaining!

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Re: For what type of dimensions should I set the parameters?

I do the same. If a dimension is going to be used in a relation or referenced in another dimension or a note, I always change its name to something like diaOuter, or lengthSlot, etc. If it's going in a family table it is a hard rule with myself that I will absolutely, no exceptions, rename the dimension to something useful. I like to say I take the time to make it easier for the next person to understand - the thing is, more often than not, that "next person" is me in the future.

 

As for the general philosophy of using relations and parameters, I like to use them to define things that I want to change in a smart way when other aspects of the design change.

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Re: For what type of dimensions should I set the parameters?

I use parameters to drive dimensions that are critical or should not be changed without understanding the model. This way, a simple click on the dimension to change it will pop up that it is controlled by a parameter. When I do this, I also will make a comment in the relations as to what this parameter means and how this dimension was calculated/controlled.

 

I also use parameters for sheet metal parts. Since sheet metal has features that are dependent on the tooling, I have parameters that control the thickness, bend radius, reliefs and other process driven geometry characteristics. In this case, I also have parameters that call out the tooling to use, which display in a drawing note. This way, I know the part can be fabricated based on the correct tooling. I can also check the drawing notes and verify the correct tooling and bend table was setup for the particular material and thickness used.

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