Inter part relations

[alvin164]

Hi guys,


I'm a newbie in Pro E WF2. I have been using UG NX3 for about 1.5 years. In UG NX3, if i want to use the length of part X in my Part Y, i can use the relations and look it up in the parameters of the other part (using wave link geometry). How can i do that in Pro E?


what i want to do is let's say my core plate's length width and height change, i want me cavity plate to follow the length, width and height of my core plate too.

thanks for the helpt

 

[vlad1979]

If you want that then I believe you have an assembly that shows the 2 parts together.


If so open the assembly, then in model tree click on the plus sign next to your first part then right_click on the first protrusion and edit, the dimensions will show, then go to info /switch dimensions. Remember the length and width, they will be like d27:16.


Repeat these steps for the other part, and you will get a dimension for second part like d15:33.


Then in assembly go to tools/ relations and write d15:33=d27:16 for the length and whatever for the width.


And regenerate and your done, remember to regenerate / saveeach part after you change the dimensions in the first part.

 

[alvin164]

If you want that then I believe you have an assembly that shows the 2 parts together.


If so open the assembly, then in model tree click on the plus sign next to your first part then right_click on the first protrusion and edit, the dimensions will show, then go to info /switch dimensions. Remember the length and width, they will be like d27:16.


Repeat these steps for the other part, and you will get a dimension for second part like d15:33.


Then in assembly go to tools/ relations and write d15:33=d27:16 for the length and whatever for the width.


And regenerate and your done, remember to regenerate / saveeach part after you change the dimensions in the first part.

Wow so much stuff to do for such a little thing....


is there another way to do it like the way i did it in UG NX 3?
or does PRO E WF2 have a better way of doing that?


thanks

 

[PRStockhausen]

In WF2 and 3 there is a relations editor that allows you to showdimensions and pick themfrom the screen.

 

[alvin164]

In WF2 and 3 there is a relations editor that allows you to showdimensions and pick themfrom the screen.

so from what u say, i'll have to have both of my plates (or parts) showing on the screen and after i click on the tools-relations, i can pick those dimensions and it will automatically update ?


thanks alot guys

 

[magneplanar]

alvin164,

It seems you want this to vary while in assembly mode. Have you considered making the component flexible? You can define dimensions you want to allow changes to and reference them to features in the assembly.

do some searching on the topic of flexible components.

not sure if this is what you need, but it works for some things.

cheers,

M


Edited by: magneplanar

 

[alvin164]

alvin164,

It seems you want this to vary while in assembly mode. Have you considered making the component flexible? You can define dimensions you want to allow changes to and reference them to features in the assembly.

do some searching on the topic of flexible components.

not sure if this is what you need, but it works for some things.

cheers,

M

hmmm no.... i don't want to make the component flexible (like spring if that's what u mean)..... I just want the plate sizes to follow each other ( what ever core plate's X, Y, Z are, i want the cavity plate's X,Y, Z to be the same...)am i making any sense here? sorry for hte confusion....


thanks for the help

 

[SRINIVASANIYER1]

Dear Alvin164,


What has been explained above are some of the possible methods. I am not very familiar about wave in UG or NX. But the following are some of the methods...


Method 1: You can create a part B in assembly mode, by referencingthe geometry of the part A. No relations needed. In this case the Part A will drive the geometry of part B.


Method 2: If you have AAX module, you can define the geometries of both Part A and Part B, in a layout or skeleton model and then drive the geometries of both part A & B thru the layout.


Method 3: Create a sketch in assembly mode. Create parts A & B using the sketch as reference. When you edit the sketch, both the parts update. Again no need for defining any relations.


Method 4: Publish the geometry of Part A and some of the references of the assembly. Reference the geometry published, to create the part B.


........Method Nxxxxxx.....


I suggest you lookup TOP Down Design tutorials available on PTC's site.

 

[vlad1979]

If I understand corectly your "wave_link_geometry" that UG does then what I described is basically the same concept, except for the fact that you manually search for the desired dimensions and not looking into a parameter list for them.


But I would go with Peter's method it's a more "few_clicks" than mine and quicker.What he means is for you to open the assembly, go to tools / relations and open the relations editor. Then just click on screen, on the protrusion from one part, the dimensions will show up, then click on the desired dimension, that dimension will be automatically added to the relations, type = after it, then click again on the protrusion from the second part, again the dimensions will show and click on the desired one and it will be added to the relations. Close the relations editor and your done.


2007-05-20_234651_relations.rar

 

[alvin164]

Thanks Vlad, SRINI, Peter and M and everyone else..... gonna try this and see how it goes....Guess i'm trully a newbie here hahahah...


cheers

 

[alvin164]

Dear Alvin164,


What has been explained above are some of the possible methods. I am not very familiar about wave in UG or NX. But the following are some of the methods...


Method 1: You can create a part B in assembly mode, by referencingthe geometry of the part A. No relations needed. In this case the Part A will drive the geometry of part B.


Method 2: If you have AAX module, you can define the geometries of both Part A and Part B, in a layout or skeleton model and then drive the geometries of both part A & B thru the layout.


Method 3: Create a sketch in assembly mode. Create parts A & B using the sketch as reference. When you edit the sketch, both the parts update. Again no need for defining any relations.


Method 4: Publish the geometry of Part A and some of the references of the assembly. Reference the geometry published, to create the part B.


........Method Nxxxxxx.....


I suggest you lookup TOP Down Design tutorials available on PTC's site.

Hi SRINI,


I just tried your METHOD 1. Is it done during the sketching mode (clicking the SKETCH, REFERENCE)?


how do i know if i have AAX module?


are there any Pro or Cons using your method 3?


Method 4 seems similar to the method i use in UG....thanks


THank You for all these tips....

 

[SRINIVASANIYER1]

Method 1: It IS done during sketching mode.


Method 2: To find out if you have AAX, File>new>Layout... If you are able to create a layout you have AAX, if not NO. (You can also ask your CAD Administrator)


Method 3: Pros: This is a simpler method. Cons: the geometries are limited to lines, circles and other sketch entities. It does not extend to surfaces. Very good for concept creation for PRISMATIC COMPONENTS.


Since the sketch is made in Assembly mode, It drives both Parts A & B. Hence the control is at a higher level. secondly creation of family of instances of assemblies along with family of instances of parts are also possible.


Good luck and welcome to PROE.