CBUSH / PBUSH

Rahul_P1

Hello together,

I have two questions concerning the PBUSH card which I am using during a frequency response analysis:

1. I tried to type in the keyword RIGID in the K field of the PBUSH card. this didn't work, so I tried the same directly in the solver deck. But I got an error message during the import. Apperently the RIGID entry is causing the error.

I read this in the userguide. What did I do wrong there?

2. Is there some more Information about the behavior of the PBUSHT card? The userguid just tells me that it is making the K entries of my PBUSH card frequency dependent. I simply like do understand what is happening there?

 

 

Rahul_P1

Student_1739

Solver decks are very sensitive to syntax and in general must be carefully edited, this as you found is the cause for the error on import.

To make the stiffness of your cbush in a particular direction to be rigid we can use the pbush property and select rigid options for that particular direction with a RIGID entry in that dof, this is done by selecting the KiRIGID option when you card edit the pbush property. see image below -

When we choose pbusht as the help says we intend to model stiffness depending on frequency, so each tabled entry in the kline of the pbusht describes how the stiffness of the cbush element varies with respect to frequency in that direction.

The CBUSH element is a generalized spring and damper. Stiffness and damping can be specified for 6 degrees-of-freedom, 3 translations and 3 rotations using the pbush or pbusht cards.

The idea behind these cards is that when you do a transient analysis you need nominal stiffness values only and these the solver can get from pbush, however when you need a frequency response analysis you will require frequency dependent properties i.e. frequency dependent stiffness in such a case you will use pbusht along with a tabled.

so let us say you are doing a frequency response analysis, and you know that stiffness of your spring varies with frequency like 25 for 1hz and 50 for 2 hz etc,
then you will create a tabled with data as 1,25 . . . 2,50 etc > refer this tabled in a particular dof in pbusht > then the frequency response run will take stiffness of 25 when the load is at 1hz etc.

Rahul_P1

could you tell me what unit I have to use for the stiffness K4,K5 and K6 in the PBUSH card?

 

Rahul_P1

Student_1739

It is the SI units, Nm/Rad

Rahul_P1

but for K1, K2 and K3 it is the linear siffness N/m correct?

 

Rahul_P1

Yes, that is correct.

 

gopal_rathore

Hi,

If we are using kN type in PBUSHT for entering the non-linear force-displacement curve, the analysis type needs to be non -linear? It is written in help file that it needs to be used only for non-linear analysis.

Altair Forum User

Altair Forum User said:

If we are using kN type in PBUSHT for entering the non-linear force-displacement curve, the analysis type needs to be non -linear?

Hi Gopal,

 

Yes, KN is allowed for NonLinear analysis.

Altair Forum User

Linear Stiffness(K1, K2 & K3) unit is N\mm or N\m?

Altair Forum User

Hi,

 

It depends on which unit you are using. If your geometry measurements are in mm then N/mm, if its in m then N/m.

 

 

Thank you