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Constraint in Rigid Sub-Assembly still affect the flexible Sub-Assembly?

Matjo

New member
Hello everyone,

In my assembly part, why flexible sub-assembly part constraints follow the rigid part. I just want to change the angle in my rigid part and after update, seem the other sub-assembly (flexible one) follow that angle.

Can someone tell me why it happen?

i very grateful for those can give me some idea ( i am newbie in CATIA :) )

p/s: sorry for my bad english :)
 

MrCATIA

Super Moderator
could you include a picture showing the rigid part and sub-assembly, and how they are constrained to each other?
 

Matjo

New member
In picture below, i want to change the angle for rigid body ( red circle diagram)

[URL=http://s1064.photobucket.com/user/matjo90/media/CATIA%20V5/Flexible%20Sub-Assembly%201_zpsumzhqcps.png.html][/URL]

So i did it, change from 40 degree to 60 degree. When i update the part, seem the flexible one follow that changing of angle and cause constraints error

[URL=http://s1064.photobucket.com/user/matjo90/media/CATIA%20V5/Flexible%20Sub-Assembly%202_zpsmhkmyyph.png.html][/URL]

Any ideas why it happened?

Thank :)
 

MrCATIA

Super Moderator
1. What is the Fixed component?

2. If I understand the sub-assemblies correctly, neither of them should be Flexible.

2a. the angular constraints between the frame/green leg and green leg/blue leg should be part of the sub-assembly

2b. and the angular constraints to the upper base should be in the top assembly

3. If you want to use different sets of rotation for left and right, then you will need two independant sub-assemblies (same set of parts, but different products)
 
Last edited:

Matjo

New member
This assembly consists three .CATProduct, where one WheelBase and two WheelAndBracket.

1.WheelBase is the fixed component. (Green plate at middle)

2.I convert WheelAndBrackets.1 (Right side) from rigid to flexible sub-assembly, and what i learned from CATIA tutorial, any changes in flexible sub-assembly do no effect the rigid sub-assembly or vice versa. In my case, i make changing on rigid one and it effect the flexible. I do know why it happen or maybe i did some mistake without i noticed.

I hope MrCATIA and others can understand what i want to say.

Thank you :)
 

MrCATIA

Super Moderator
Instead of having us guess at what parts are instanced and what part is constrained to what part, could you please expand your tree diagram and attach a copy. I'd like to see the constraints in all assemblies, and all the parts.
 

MrCATIA

Super Moderator
Thanks for the pictures. now I can see the complete assembly structure.

1. Again, I don't understand why you are using Flexible sub-assemblies. All of your assemblies are fully defined within themselves, and do not need to be constrained to features in a higher assembly. Rigid sub-assemblies will work for this.

2. Angle.12 and Angle.13 (10° and 20°) can be different because they control two different sub-assemblies (WheelAndBracket.1 and WheelAndBracket.2). This is good.

3. There is a 45° angle and a 35° angle that are conflicting, since they are in the same sub-assembly (BracketArms) that is instanced twice. If you want to use the same sub-assembly, it must have the same constraints.

4. same as comment 3: There are two 60° angles in the WheelAndBracket sub-assembly that is also instanced twice. These angles should always be the same if instancing the same sub-assembly. If you want these angles to be different, then you need a second WheelAndBracket sub-assembly (but with a different name) that can have different contraints.
 

MrCATIA

Super Moderator
I just noticed that Angle.12 is wrong. It should be between WheelBase and WheelsAndBrackets.1
 

Matjo

New member
Dear MrCATIA,

Actually this assembly is one of my tutorial exercise that i use for my learning material in CATIA. So, on that exercise, the creator exercise shown he can change that angle ( angle which is i had been asked in this post) while i can not do it. Although i had follow the tutorial step by step without changing any method. This is main purpose why i asking some idea from MrCATIA and others because i curiosity to solve this problem. Maybe for next future, i will face this problem again. Just want to increase my knowledge in this CAD software.

Thank you MrCATIA because always keep reply my question :)
 

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