Cancel
Showing results for 
Search instead for 
Did you mean: 
Highlighted

Contact/bolt pre-load in SOL103

Experimenter
Experimenter

Hi All,

 

I created an example to learn about bolt pre-loads and contact with Modal analysis.

 

Image 1. Two rings  grey is aluminium, green is ABS, bolted together with 5 symetric bolts.

Image 2. SOL101 to show bolt pre-loads and face to face ring contact applied correctly.

Image 3. SOL103 (with static sub case, pre-loads and contact). Defined STATSUB = 1 in Subcase - Eigenvalue Method 1 case control user keyin text.

 

Bolt pre-loads correct (no penetration at bolts locations) but Top ring penetrates bottom ring between bolts.

Obviously not possible in real life!

 

Any help very much appreciated.

NX11 files attached.

 

 

 

BoltedRings.PNGgeometry
 

BoltedRings von Mises.PNGSOL101 Bolt pre-load and surface to surface contacts

 

BoltedRings SOL 103 With bolt preload and contact static case.PNGSOL103 with static case for pre-loads and contacts

$*$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
$*
$* CASE CONTROL
$*
$*$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$
$*
ECHO = NONE
SPC = 1
BCSET = 100
OUTPUT
DISPLACEMENT(PLOT,REAL) = ALL
FORCE(PLOT,REAL,CENTER) = ALL
SPCFORCES(PLOT,REAL) = ALL
STRESS(PLOT,REAL,VONMISES,CENTER) = ALL
$*  Step: Subcase - Statics 1
SUBCASE 1
LABEL = Subcase - Statics 1
LOAD = 4
BOLTLD = 3
OUTPUT
DISPLACEMENT(PLOT,REAL) = ALL
FORCE(PLOT,REAL,CENTER) = ALL
SPCFORCES(PLOT,REAL) = ALL
STRESS(PLOT,REAL,VONMISES,CENTER) = ALL
$*  Step: Subcase - Eigenvalue Method 1
SUBCASE 2
$* KEYIN TEXT
STATSUB = 1
$*
LABEL = Subcase - Eigenvalue Method 1
STATSUB = 1
METHOD = 102
$*
$*$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$$

3 REPLIES 3

Re: Contact/bolt pre-load in SOL103

Gears Phenom Gears Phenom
Gears Phenom

Hi Martin

 

The key thing to understand here is what stiffness matrix nastran is using to calculate the modal eigenvalues.

 

It is using the last updated stiffness matrix from the SOL101 and does not update at any point during the modal extraction.

 

So, if you look at your SOL101 contact pressure you will see that there is no contact - other than around the bolt hole areas, which means when nastran starts running the modal - it will not see these areas as "in contact".

 

CONTACT.JPG

 

Part of this is due to the use of RBE3s at the bolt location and not including the area of washer/head/nut. I have modified the input deck to use RBE2s and include this area - as there will be some stifness all rotations are free as the head etc. can "roll". below is my contact pressure:

 

CONTACT2.JPG

 

As you can see, the model now has some (albeit small) contact pressure at the intermediate points. Nastran will now see these as "in contact" when outputting the stiffness matrix and hence my modal has no pentration at these locations:

 

MODAL.JPGYou will notice than penetration occurs where the contact pressure was zero:

 

MODAL2.JPG

 

Play around with your bolting arrangement and update the Rigid Elements to include the stiffness and area from head/nut bolt and you will convergence on a full surface contact solution.

 

Hope that helps.

Stuart

Re: Contact/bolt pre-load in SOL103

Siemens Phenom Siemens Phenom
Siemens Phenom

Stuarts reply is right on. The modal solution is purely linear. The final converged contact stiffness from the static subcase is used in the modal case. In this sense, the areas in contact become glued and the other areas are unconnected.

 

The green ABS ring is so thin that I doubt that there is anything you can do to this model to get it to seal all the way around. It will need to be thicker or have ribs added to increase the effective clamping radius of the bolts.

Re: Contact/bolt pre-load in SOL103

Experimenter
Experimenter

Thanks for the tips!

 

I played with the model, increasing the bolt/nut surface areas and using RBE2 elements instead as recommended.

Penetration was reduced in some modes but not others as I was not able to get contact pressure all the way across the face between bolts (even by thickening the ABS to be the same as the ALU).

I tried adding gravity and a pressure sim object to make sure there was contact between rings but no joy (it also introduces stresses that aren't present in practice too).

 

Another thought was to create a Manual Coupling between ring surfaces and fix DOF3 to make sure the ring face move together. This was the most effective for the modal results but is still not corect behaviour as it behaves as if the surfaces are glued.

 

I'm not sure it's possible to model this senario with the limitation of solved linear contacts as input to the modal analysis though. My only thought was to do the study with SOL 601 but it's the frequency response I am interested in (at what rpm will the ABS ring flex up and break).

 

I was able to make the model much better with your recommendations thanks. I will keep working on it!