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How to construct a shell with inside the driven dimension?

bhayden

New member
I'm got a cube I'm turning into an open box using the #insert #shell Feature. This leaves the outside dimesion of the cube (created with as a solid protrusion) driven by the outside dimension of the cube. Is there a way to create a shell feature such that if you change the thickness the inside of the shell stays the same? I'm doing this in 2001 Foundation II package.



Bernie Hayden

XKL LLC
 

kschubert

New member
Not sure what you mean, but I've created covers by taking the solid and then giving the shell a negative thickness (so the inside always matches the mating part)



Would that work for you?
 

bhayden

New member
I gave that a try expecting it to fail. It actually works as long as you use redefine as opposed to modify. That sort of worked except then I discovered that in one direction the important dimension was to the inside and in the other direction the important dimension was to the outside.



I think the answer is to learn about surfaces.



BTW, this whole exercise is to create imaginary modules that mark out space claims and assembly constraints in the early phase of a project. Working only with the Foundation II module I'm not sure how much of this will carry forward in a true Top Down Design but at least it creates a working document to reference from at the begining.



Some of the copy geometry functionality is added to the Foundation II package when you install the Wildfire license. Supposedly Skeleton functionality isn't available. Maybe it's because I use a _skel part as a start part or possibly just because of the file naming convention but it seems to work. That is the skeleton models aren't shown in the BOM.



-Bernie-
 

dr_gallup

Moderator
The easiest thing to do is create parameters for the dimensions you want to control (inside_width, inside_height, etc.) and then write relations between the parameters, shell thickness and outside dimensions.
 

bhayden

New member
> Replied by dr_gallup on 12/17/2003 4:11:00 PM

> The easiest thing to do is create parameters for the dimensions



I'm not seeing how this can be applied. If the driven dimension is outside and you want to see an inside dimension you can't change the references with parameters. If you create a reference dimension to the inside it'll automatically update if the thickness changes so why express it as a relation? A reference dimension would work for showing design intent on the drawing; which is the main point behind this exercise. However, it would be nice if it could be the driven dimension.



-Bernie-
 

kvision

Moderator
I created a rectangular box. I used a shell with neg thickness. All of the dimensions refer to the interior dimensions of the box. I can easily modify the thickness without redefine. i am using pre/e 2001 build 2003320.
 

dr_gallup

Moderator
Parameter:

Inside_dim=12



Relation:

Outside_dim=Inside_dim+(2*shell_thickness)



Now you can't modify Outside_dim directly, if you try to Pro/E will tell you it is controlled by a relation. Show the parameter &Inside_dim on the drawing and modify that and dimension shel_thickness. The Outside_dim will update when you regen.
 

bhayden

New member
Ah, now I think I understand. The parameter Inside_dimension would be shown as a note rather than a dimension. There's no way to make it so that you can modify the parameter from the drawing is there? It would be nice if the note showing the parameter Inside_Dimension was displayed like a dimension but I don't think this can be done either. It seems that even if you insert a reference dimension and replace the text with a note the dimension value is automatically added back to the dimension text.



So what I ended up with was a Parameter INSIDE_DIMENSION = 17.00 and I expressed the width of the cube as d1=2*d4+INSIDE_DIMENSION where d4 is the dimension governing the thickness of the shell. I'm surprised that this worked since d1 is in a feature prior to the shell deing defined. Probably not great modeling practice.



-Bernie-
 

bhayden

New member
For this particular part that would have been a better way to model it. However, the dimensioning issue would be the the same. That is all the driven dimensions would be either inside or outside (or centered I guess) but to show design intent I need the width to be an inside and the height to be outside.



Using parameters and relations does the job from a modeling point of view but it's not possible to create a drawing where you can change the model with driven dimensions



-Bernie-
 

dr_gallup

Moderator
This might get blasted in the Good Modeling thread but it works:



Make the parameters and relations as in my post above.

Create a driven dimension for the inside. Add a dim related note with the text &inside_dim and place it related to the driven inside dimension. Modify the text height of the driven inside dimension to 0.001. Voila, you can now pick modify and choose the parameter that looks like a dimension.



Where there's a will there's a way!
 

bhayden

New member
> Modify the text height of the driven inside dimension to 0.001



I actually thought of this too, I'm embarassed to say ;-) It doesn't really accomplish much though. First of all the note can not be part of the dimension text or it gets scaled down too. So there's no associativity between the dimension arrows and leaders and the parameter note. Second, there's no way to change the parameter value in drawing mode, you have to open the part.



BTW, any time you open the Properties dialoge box for a dimension it automatically resets the text height to the default. At least that's what happens in 2001, I assume Wallflower does the same?



-Bernie-
 

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