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KEEP FLEXIBILTY ASM&PRT

bonar

New member
Hello. l have perhaps basic question...


PROBLEM: How could lcreatea flexible part in assemblly and keep him flexible in part too?


lHAVE MADE:l created a part and than l inputed them into assembly and on assembly level l defined flexibility. BUT thes flexibility isn
 
Why would you need a flexible part in part mode? The point of flexible parts is they are manufactured to a certain size, i.e. the free length of a spirng, the free state of a rubber pad, etc., and the part drawing details them in that free state.


Of course, you then fit them to an assembly and the flexibility is required to fit them, e.g, a compressed spring. The part can be used in multiple assemblies with differing dimensions in each, without affecting the manufacturing detail of the part.


At the part level it is flexible anyway because you can simply modify the dimension to whatever you want it to be. If you are talking about having various sizes of a part, maybe you need a family table, e.g. different lengths of a screw. If you change the basic size of a part in it's free state you affect it's fit/form/function and should have a different part number for each instance.


Maybe if you described how you would apply part flexibility at the part level we may be able to help?


Regards,


David
 
I understand you flexibility need ...


You are in the design process and you want things to move between the assembly and the part ... or versa visa ...


First you need to plan a strategy on which one you want to remember that has the relationships in it ...


Generally I know the part or parts that are going to flex the most. So I design all parts in the assembly mode, even the the cuts& protrudes.


Just activate the part in the assembly and create a sketch and use/offset edges and/or create concentric circles. Now all of the relationships are being stored in the assembly file, which you must remember. I usually name those assembly files 'design-aids.asm'.


Once all of the design is done, then you must open each part file and select each feature and unalign them from the other parts or assemblies and dimension them.
 
dakeb1 said:
Why would you need a flexible part in part mode? The point of flexible parts is they are manufactured to a certain size, i.e. the free length of a spirng, the free state of a rubber pad, etc., and the part drawing details them in that free state.


Of course, you then fit them to an assembly and the flexibility is required to fit them, e.g, a compressed spring. The part can be used in multiple assemblies with differing dimensions in each, without affecting the manufacturing detail of the part.


At the part level it is flexible anyway because you can simply modify the dimension to whatever you want it to be. If you are talking about having various sizes of a part, maybe you need a family table, e.g. different lengths of a screw. If you change the basic size of a part in it's free state you affect it's fit/form/function and should have a different part number for each instance.


Maybe if you described how you would apply part flexibility at the part level we may be able to help?


Regards,


David


Thx you Dakeb1 for some new ideas. l
 
tosh382 said:
I understand you flexibility need ...


You are in the design process and you want things to move between the assembly and the part ... or versa visa ...


First you need to plan a strategy on which one you want to remember that has the relationships in it ...


Generally I know the part or parts that are going to flex the most. So I design all parts in the assembly mode, even the the cuts& protrudes.


Just activate the part in the assembly and create a sketch and use/offset edges and/or create concentric circles. Now all of the relationships are being stored in the assembly file, which you must remember. I usually name those assembly files 'design-aids.asm'.


Once all of the design is done, then you must open each part file and select each feature and unalign them from the other parts or assemblies and dimension them.


Thx for response.l don
 
Create part #1 and extrude a cylinder feature.


Create an assembly and assemble part #1.


Create new part #2with just datums and assemble it tothe assembly. Activate it.

Extrude a cylinder, where you select the top surface of part #1 as the sketching plane.
- Now you are in the sketcher.
- Create a larger circle concentric to the part #1 cylinder.
- Dimension it from the quadrant of part #1 cylinder to the same quadrant of part #2 circle.


View attachment 4671
=============
-Extrude part #2 to some positive height.


View attachment 4672


=====
Now go to the tree list view and activate the assembly again.


=====
Go modify the height of part #1 and regenerate and watch part #2 move when part #1 changes.


View attachment 4673


=====
Now change the diameter of part #1 and regenerate and watch part #2 diameter size change also.


View attachment 4674


Please remember that you have constructed a parametric relationship between two parts in the assembly mode and when you save the assembly file the relationship is stored in the assembly file.


Open part #2 and edit definition, enter the sketch and remove the alignment of the circle from part #1, remove the 5.85 dimension,thendimension the diameter of the circleand then constrain it in the x,y with dimensions. Exit the sketch and go to the assembly and modify the part #1 diameter and notice that part #2 does not change size anymore.


=====
Hopefully you see that you can design products quickly in the assembly mode and build relationship dimensions referencing features of different parts.


Then when you change a dimension in one part, the other part will change in size, where it keeps the same distance, such as 5.85 offset.



Edited by: tosh382
 

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