Changing part position in an assembly?

[Pentatonic]

Hello All,


I have an assembly of 3 partsand would like to be able to move one part to different positions for some different design ideas. In IDEA-S, I could simply specify an axis as the direction I wanted the part to move in, and a distance, and I was done!


But I have Pro/E Wildfire 2.0, and the help menu tells me I can move a part position by going INSERT->COMPONENT->PACKAGE->MOVE, but the darn "MOVE" option is grey and I cannot select it no matter what I do!

Does this mean I need a stupid Ad-on module that will cost me more money, or is there another way to do this? Please keep in mind I am a total Pro/E newbie and only started learning and using it 2 days ago.


Thanks!

 

[AHA-D]

The most obvious way is to change the relations. When parts are in a particular position in regard to the other parts, you can either change distance parameters, or exchange one relation for another. You could make a family to keep all of the different configurations alive.


Alex

 

[trillicomm]

Create a Family Table in the assembly and select the placement dimension that you want to move, make sure it's an OFFSET (not a coincident or oriented) so you can specify a new number for each instance.

 

[Pentatonic]

Is there any other way to do it? The help menu seems to imply that I can only create table drivenPARTSunless I havePro/ASSEMBLY:







Module

Available Family Table Functionality


Basic Pro/ENGINEER

Create table-driven parts by adding dimensions to the Family Table



Pro/ASSEMBLY

Create table-driven assemblies by adding to the Family Table subassembly and part names, as well as assembly dimensions.

 

[trillicomm]

what you found there is the best way

 

[AHA-D]

You don't need to create table driven parts when only their position changes. Correction : you might need to do so if you want to use varying datum planes in parts to build assembly relations.


But in your case you're probably best served by creating an assembly and copy it to another filename, after which you change the parameters in the new file. Each assembly file will show another configuration of the design.


Alex


PS : This ProE thing where you always seem to need a module that you don't have sucks ...

 

[mcgowanp]

This may be specific to Ideas, I cant remember as it is years since i used it but check the part or parts that you want to move. If the component is fully constrained i.e. that is has no remaining degrees of freedom. If you want to be able to move a component is the z direction the make sure that it is constrained in the x and y and not in the z, you will then be able to drag it in this direction.

 

[vlad1979]

2 days hmm

, I remember the excitement and frustrations when I started with PRO_E.


If you want to move a part to one direction,right_click onethe part you want to move / edit definition and the window below will apear.


View attachment 3340


Now look at all the constraints, click on them to see what each of them do. Locate the one that constraints the part in the direction you want to move. For example I have acover with 2 holes that is assembled on top of a part, with the constraints above insert hole -hole and mate the cover surface and housing surface.


Let's say I want between the cover and housing to be a little gap. The constraint in that direction is controlled bymate so I give a valueof 20mm and hit enter to move in one direction. If I need it moved in the opposite direction Ienter -20mm.


Now, if you want to move the part freely in that direction, delete the mate constraint(just click on it in the window above and then click on the red "-" sign) then click on the move tab, then translate , then click on the arrow indicated, then click and release somewhere on your part, then move the mouse. The part should now move freely in that direction. When your happy with the new position click again and the part will be released in the new position. But the component is now "packaged" that means it's not fully constraint. So click on the place tab and add a new constraint mate (the previous you delete).


View attachment 3341


If you want to freely move a part in all directions you must first delete all of it's constraints from the window above (don't close the window)and then:


-hold down both CTRL+ALT and then with middle mouse button you rotate the part


-hold down both CTRL+ALT and then withright mouse button youmove the part


And also see these:


http://www.me.cmu.edu/academics/courses/NSF_Edu_Proj/Wildfir e_short_course/tutorial8.htm


http://www.me.uvic.ca/~mech410/ProE_Lectures/5%20Detailed%20 Instruction%20on%20ProE%20WF2.pdf
Edited by: vlad1979

 

[Pentatonic]

2 days hmm

, I remember the excitement and frustrations when I started with PRO_E.

THANK YOU for the informative post!

Yes, 2 days, so I don't even quite know what it means to "change a parameter" let alone how to do it haha, so I like screen-shots and arrows!

Well, this is my 3rd day learning, so I'm gonna give your method a try this afternoon...

 

[AHA-D]

ProE definitely is NOT a program you can start learning by just clicking around and having no written guide at hand.


I started ProE with something like 15 years of previous CAD experience, everything from electronic drawing board to full parametric 3D, so I thought "it can't be that difficult to get this new thing going" ...


Well ... I was wrong

It took me about 3 months to get "the hang" of the ProE philosophy and 6 months to dare to call myself professional again.


Alex

 

[verge]

Pentatonic,


I started in I-DEAS, also, and have also worked extensively in Unigraphics, and can tell you that, although there are many similarities, Pro-E is definitely a world unto itself. Becoming comfortable with constraining and moving the parts of your assemblies around seems to be a really important part of becoming fluent in Pro-E. Just whip those constraints out of there when you need to. Be sure to think about how you're constraining the parts, and think visually. Vlad has you set up with some excellent information on these things, just become confident with these techniques and it will all seem a lot easier.


I would probably copy the file with another assembly name and simply remove your part's constraints and replace them with new ones, or offset them to where you want them to be.


Welcome to the forum...