Very simple usage of Parameter

[KevinMacDonald]

Suppose I am building a simple frame - a cube - consisting of edge members that define the exterior of the cube. I define a length of one side of the cube as a user parameter. Call it parameter 'x'. Now, I create a sketch of a profile and I want to extrude the profile. The length of the extrusion I want to be controlled by parameter x. Perhaps it is x - 3in. I am finding that when I extrude the sketch I am not able to enter a parameter as the distance of the extrusion. What am I missing?

Thanks

[ystrm]

Not really sure what you are missing here.

But my way of doing something like this is:

-Create a sketch, draw a rectangle, when dimensioning one of the sides, i type in "X=5 in", then the parameter X is created.

-Extrude the rectangle to a cube, when typing in the length, then write "X-3 in".

Another way of doing it is to open your parameters tab, after extruding your cube, look up the parameters, change the name and equations for it.

I hope that helps you.

[Logos_Atum]

Have you tried to list the parameters in the extrusion tab.

That way it´s easy to see which parameters and if other

parameters would be accepted by the extrusion itself.

Are you generating parameters in the sketch already and

how are you doing it?

I generate them by typing length=50mm for example.

Not sure if i got you right but it´s supposed to work if the

parameter is listed in the extrusion tab.

Looks like it looks on the attached screenshot but certainly

not in German 😉

[swhite]

When you add the dimension you type your parameter, not your value. If you have the paramter set already as x, then type x in the dimension, Or you can simply type x=3 and the parameter will be named x. In sketches. In extrusions there is an option on the drop down entry box that allows you to list all parameters and choose one.

[KevinMacDonald]

I am definitely missing something. I suspect it is some fundamental principle of how parameters work.

When I started my new assembly I created some work planes which are at the top level of the hierarchy in the browser. Working at that level I created a user parameter and called it 'x'. I use x to define offsets for those work planes from the origin work planes. That works fine. Then, I created a new part. When editting the extrusion of that part the user parameter 'x' is not available!! If I type x or x-3in as the length of the extrusion it shows as red, meaning Inventor cannot parse the equation. It appears that not all parameters are available all the time to all objects. Is this true?

I don't see how any of this has anything to do with sketches. The extrusion happens after the sketch has been completed. 

Thanks

[Curtis_Waguespack · Accepted solution]

Hi KevinMacDonald,

It sounds like you're attempting to use a User Parameter defined in one file (the assembly) in another file (the part). You need to link the parameters in order to use them across files.

However, if you attempt to link an assembly parameter into a part that is used in that assembly, it will create a cyclical relationship and will not be allowed. You can however, link a parameter from one part to another part, and use them both in the assembly.

http://www.youtube.com/watch?v=qvIR5TQ6OvI

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[KevinMacDonald]

I also tried linking parameters from the part where the extrusion is from the parent assembly. Inventor through an error saying that would cause a cyclic dependency. Definitely missing something fundamental. 

My objective I believe is really very simple. I want to parametrically control the length (ie the extrusion distance) of a part used to construct an assembly that is basically a simple box, using a parameter that I have defined for the length of the box. That's it. 

Thanks

[mrattray]

Assembly parameters are not available to it's parts. The best way to overcome this problem is to model your assembly as a multi-body solid. Otherwise, you'll have to use iLogic.

[KevinMacDonald]

Whoops. I only just saw the above reply. I will try that.

However, I am confused by it. It seems very natural to me, at least, that parameters defined on an assembly might be used to control parts within that assembly. It sounds like I need to create a dummy part whose sole purpose is to define geometry of the overall assembly, and then link parameters from it to other parts. 

I think I am looking for a design pattern or methodology that helps to frame my thinking on this subject.

Thanks

[mrattray · Accepted solution]

That's called "Skeletal Modeling" and can be a very powerful technique! I actually recommend that you look into both skeletal modeling and muscular modeling (multi-body solids). Both techniques are described in AutoDesk tutorials.

[KevinMacDonald]

Still working on my very very simple parameter exercise. Inventor has offered me another puzzle.

If someone doesn't mind, please download and unzip the attached file containing an assembly and a few parts. One of those parts is called SharedGeometry. Notice it has a Parameter called side_length, and a work plane called Work Plane8. Try editting the dimension of that plane. Select side_length from the ListParameters dropdown. Either use that parameter, or do what I was doing and enter side_length/2. Finish the edit.

Now, edit the dimension again. Note that whatever you entered is poof gone.

What I am trying to do is create a series of work planes offset from the origin planes. Each is offset positive and negative by (side_length/2) in order to form a cube. I will be using those planes to constrain parts such as the EdgePiece part. Note the length of the extrusion of EdgePiece is set to side_length - 6in. That works OK. But, for some reason I cannot create my work planes using that parameter.

Thanks

[mrattray]

Works for me. Try a reboot?

[swhite]

A simple solotuion, have left the sketch visible for clarity. Attach workplanes to sketch lines using the orgin planes for alignment only. Can be changed by a simple dimension or parameter update. Use this now and then when I need workplanes that easily adjust without having to adjust each one seperately.

[KevinMacDonald]

Parameters are slowing making more sense. I get the feeling that a decent approach would be to have a couple of "phantom" parts in my assembly - one for containing parameters to be shared throughout the assembly, and perhaps another for containing work features, planes, points etc.

Thanks for all the suggestions.

[dano0310]

Can you use excel for the parameters that might be easier.