How to show component location dimension?

[bhayden]

I have a series of components I've located by mating two surfaces and then offsetting datum planes by a set amount. How do I get these offsets to show as dimensions on the Assembly Drawing?



Bernie Hayden

XKL LLC

 

[Guest]

In the drawing, try right-clicking on the features/components in the model tree and pick something like Show Dimensions (don't have Pro/E in front of me right now, but it's something like that).

 

[bhayden]

> right-clicking on the components in the model tree and > pick Show Dimensions



This only shows the dimensions that describe the component (i.e. it's dia, height, etc.). What I want to show is the assembly dimensions which are offset planes.



The other glitch with this method is that ALL the dimensions are inserted without the chance to select which ones you want to keep or erase.



-Bernie-

 

[Guest]

Yes, you're right about that. You'd think it would give you assembly level dimensions.



I am able to show assembly constraint dimensions (mate offset, align offset, etc.) by using the Show/Erase dimensions dialog box. Selecting Show By View or Show All displays the assembly dimensions.

 

[bhayden]

I thought I'd figured it out after reading looking at my last response.



> I want to show is the assembly dimensions which are

> offset planes.



I figured that having the planes display turned off it wasn't showing me those dimensions. I constructed a simple test assembly (a small block stack on top of a larger block) and that proved not to be the case. The only thing I can find that works is to essentially do a show all for the view you want the assembly dimensions to appear in. Kind of a brute force method since you can end up with hundreds of dimesions to sort through.



> You'd think it would give you assembly level

> dimensions.



You' think! I can't seem to find any way to filter for this by assembly constraints or by feature (picking the datums used for assembly). I have the feeling I'm missing something.



-Bernie-

 

[Tunalover]

Guys-

Just do sketched dimensions from the component edges to whatever edges you want. Is this solution too simple?

Tunalover

 

[donha]

This is the Pro/E 2001 approach. I have placed the Show/Erase icon in my menu. If you have not, choose View/Show and Erase. Highlight the dimension Type, I normally choose Show By Feature and View. Next choose Sel by Menu and choose the viewport you wish to show the dimension in. The Selection Tools Menu pops up. The default is to show (Look In) and the assembly will be default. Choose Select All and and your dimension will probably appear. If not, know what feature number to choose. The same works in reverse for showing component dimensions on the print. When the Selection Tools pop-up box appears, choose the arrow on the Look In option and choose a part. The dimensions will now show for that part only. Hope this helps.

 

[Guest]

Tunalover - A created dimension would work. Just remember that you would loose associativity between the assembly and drawing (i.e. you could not modify the dimension from the drawing and have it update the assembly). If you don't really care about this functionality, then your way would work...



P.S. Created dimensions vs. Shown dimensions would create an endless debate!

 

[bhayden]

I'd originally resorted to using a created dimension. However, when possible I really try to focus on design intent when creating the model so it seems a shame to throw away that work.



I guess my only gripe is that it seems you have to do a show all to get the assembly dimensions. This can sometimes result in so many dimensions splattered on the screen that nothing is legible. It seems there should be some way to filter just the assembly dimensions.



-Bernie-

 

[Tunalover]

Jason and bhayden-

Occassionally one should step back to look at the forest. Is it really worthwhile having shown dimensions in this case? I think that this is one of those times where it DOESN'T REALLY MATTER. As CAD users, we often spend more time on the tool than on the design. Let's not become slaves to the tool!



Bruce

 

[bhayden]

Bruce,



In this particular case the assembly is a first guess approximation for a prototype. At this stage the drawings are as much for my benifit as a designer as they are for future production. Using shown dimensions acts as a design check and since it's quite likely the dimension will have to be adjusted it's much easier to have the number on the drawing than to have to go back later and interogate the model. Open the drawing, enter the redlined values, save, print, done.



If the tool is too cumbersome to use in this manner then so be it. But if the capability is there and can be used with a little up front effort why not use it? In this particular case Show all produced just the dimensions I was looking for. That was largely because other dimensions on the drawing had already been placed. If there are other (better?) techniques for isolating assembly dimensions the knowledge will likely be of value in the future when the assembly is much more complicated.



Bernie Hayden

XKL LLC

 

[donha]

Best practice where I work is to show driving dimensions on the prints. This way you do not have to figure out what feature to change, you do not have to call up the model and your changes are quick and easy. Personally, I think it is crappy work to create dimensions on a print when you can have the models dimensions on the print. Just my humble opinion . BTW, we paid a vendor $5000 to create a complex model and print for us. When I got the print, ALL dimensions were created dimensions. I took the time to model the part and create a new drawing. $5000 down the drain. Lesson learned