Bolt pretension in radioss

Hi,

I am trying to load a bolted structural model and assign pre-tension to the bolt. I have made a spring element connected between two solid parts of bolt. I can see that pretension can be assigned using spring 13 property and also type 32 spring property. In type 32, what so we mean by Stif0 value? Also how to assign pre-tension using both?

Thank you

Find more posts tagged with

English

Radioss

Accepted answers

All comments

Altair Forum User

Hi Gopal,

As you can see in the Help menu Stif0 is the spring stiffness before sensor activation and unloading stiffness after sensor activation. A time sensor is created and and is recalled in the sensor of the property card. As soon as the time specified in the Tdelay is reached the spring will act based on the the force vs displacement function the user specify. This Stif0 value will be the spring stiffness value as soon as the sensor is activated. Please go through RD-T: 3510 Cantilever Beam with Bolt Pretensioner tutorial in Help Menu. I'm attaching a document also oo the RADIOSS elements where pretension spring is also covered.

You can apply pretesnion in Type 13 spring also. Create a function accordingly and assign the same, that is you can load it from time 0 so that the spring will be under pretension. I'm attaching a sample model file for your reference, In the functions please check the curve defined.

Unable to find an attachment - read this blog

gopal_rathore

Hi,

The curve is as follow in above files:

X Y

-3.0 ,0.0
0.0, 10.0
3.0, 100.0

This is a curve between force (Y) and defleciton (x) right, i am seeing this as per help file.

Thank you

gopal_rathore

Hi @George P Johnson

Kindly let me know about this.

Hi,

The curve is as follow in above files:

X Y

-3.0 ,0.0
0.0, 10.0
3.0, 100.0

This is a curve between force (Y) and defleciton (x) right, i am seeing this as per help file.

Thank you

Altair Forum User

Hi Gopal,

This is Force vs Displacement curve.

gopal_rathore

Hi Gopal,

This is Force vs Displacement curve.

Hi,

So is it -3 mm displacement at 0 kN force . Does not this look like any problem in this?

If it is displacement with time, then at t=0, it under with pretension of 3 mm and then as time increase bolt loosens .This seems ok.

Kindly clarify .

Thank you

Altair Forum User

Hi Gopal,

This if Force vs Displacement only. For example purpose these values were used.

Negative values in displacement indicate compression and positive shows tension. As per the curve when the spring is compressed 3mm no force is acting on it but when the spring is at its original state, ie 0, it has a force of 10N thereby making the spring pretensioned.

gopal_rathore

Hi,

Thank you for the update. In property spring 13, we have K_tens and then we have function ID for stiffness curve. If we have the curve, then we can have K_tension as blank right?

Altair Forum User

Yes, you can leave it blank.

gopal_rathore

Hi,

I am working on a model having M16 bolt (having tightening torque of 250 Nm and thus pretension force of around 80 kN.I ahve used the following curve for bolt pretension assigned to type13 spring property.

x y

-1.0 78000

0.0 78000

1.0 88000

As the bolts is under pretension right from start, the energy error starts from -99 % and gradually reduces to -1 % to 4 %

This is only happening when I am using pretension force of 14 kN and not exact value of 80 kN

On using higher pretension force value, the energy error does not redcue from -99 % and the bolt made by 3D elements is getting deleted.

Is this due to high pretension, force or anything else?

I have send the files through secure link.

Altair Forum User

Hi Gopal,

This energy error seems to be because of the bolt pretension.

We will check the model and will update you on this.

gopal_rathore

Hi Gopal,

This energy error seems to be because of the bolt pretension.

We will check the model and will update you on this.

Ignore the first file send.

I have resend it again. Kindly consider the new one.

Thank you.

Altair Forum User

Hi Gopal,

Reviewed your model.

It seems like there is some high hourglass energy in the model. Please keep N=5 for shell elements and Isolid=24 for solid elements.

There are many penetrations in the solver interface. Please correct them

Finally, the model has high contact energy.

Set “physical” contact interface gap value. Slightly increase the Gapmin value also. And use the recommended parameters for the interface and also check the master and slave material characteristics.

gopal_rathore

Hi, the attached graphs are coming for me.

For higher pretension force, the above said thing is happening.

<?xml version="1.0" encoding="UTF-8"?>

gopal_rathore

Hi,

Please find the attached image . In this, there is penetration between two plates connected at nodes i.e no free edges in between. The penetration is coming due to large thickness value I think

How can this be avoided here.

<?xml version="1.0" encoding="UTF-8"?>

Altair Forum User

Hi Gopal,

Normally for pretension cases high negative energy error will be there during the starting of the run and it reduces gradually. But in this case for very high pretension forces high energy errors are coming, it reduces and finally it again goes up. It seems like it is due to this high force.

The only possibility for the above case is to create connectors. You may have to delete one or two element layers of 12mm plate and use connectors for establishing the connection.