GAP elements

[janipk]

Hello to everyone,

Could anyone give me some information about 1-D GAP elements i.e what they do? how can be modeled? Are they can be used in linear calculations also?

Thanks

 

[Onda]

Linear Gap are useful for easy contact problems. To model them there are in Patran some utility.
They must be used in linear calculation with param CDITER.
The solver make iteration until all gaps are resolved (no change in gap condition between two iteration).

You can find in this paper what you could do with linear gaps:

http://www.mscsoftware.com/support/library/conf/auc99/p05799.pdf

You can check also this tread :

http://www.eng-tips.com/viewthread.cfm?qid=178285&page=1

Regards
Onda

 

[janipk]

Hi to everyone,

thanks to Onda!

I have modeled the gap elements and have strange results.
Actully I have a cylinderical shape model having some parts inside which have contact with the cylinderical part.

I modeled the linear gap elements between them. I have pressure acting in the radial direction and some spcs as boundary conditions. It seems that everything working nice i.e iterations are being performed but don't behave like that they have no contact between the parts.
I have defined the dof's of coressponding nodes in radial direction, which means that I have the orientation of gap element in radial dirction(not sure)e.g.

SPOINT 4611350 4611351
SUPORT 4611350 0
SPC 101106 4611351 0 0.5
MPC 101106 280 1 1. 586 1 -1.
4611350 0 1. 4611351 0 -1.

I have checked with a simple model (two plates 100mm in X-axis 10mm in Z-axis having gap of 0.5 between them) having gap elements and having pressure applied Y-axis dirction.
this model working nice. e.g
SPOINT 4611350 4611351
SUPORT 4611350 0
SPC 101106 4611351 0 0.5
MPC 101106 280 2 1. 586 2 -1.
4611350 0 1. 4611351 0 -1

but with first model it don't. Is there something wrong with the orientation of gap element in cylindrial coordinate system?

Looking forward for you kind suggestions!

thanks

 

[Onda]

Hi ,

I have used Linear gaps in Cylindrical Coordinate System and they work pretty well.

My suggestion is to always use not coincident nodes in way that you know in which direction you have contact.

You should also define both nodes pair in the same coordinate system.

I have modeled a pin - hole problem and the load pattern and contact area was perfect.

Onda

 

[janipk]

Hi,
Thanks Onda for your information!

I have non-coincident nodes and there is gap of 3.649902 e.g

$gap between grid 331869 dof 1 and grid 460605 dof 1 init opening = 3.649902
SPOINT 4611352 4611353
SUPORT 4611352 0
SPC 101106 4611353 0 3.649902
MPC 101106 460605 1 1. 331869 1 1.
4611352 0 1. 4611353 0 -1.

Could you please let me know about:
SUPORT 4611352 0,
what does shows 0 here, is it Coordinate System ID?

Is it possible for you send me an exampler input file?

Thanks in advacne!

 

[Onda]

Janipk,

The 0 in the SUPORT entry mean that 4611352 is a scalar point and not a grid point. Else that integer should be the degree of freedom of rigid body motion.
I think you should try with a much smaller gap. I don't know dimensions (and units) of your model but a gap like 1/10 of mm should be better.
I will look for an example model but It will take me some time.

Regards

Onda

 

[janipk]

Hi Onda,

Thanks! I have tried everything but in vain.

Anyhow waiting for your your example model modeled in cylindrical coordinate system.

Regards,

JOnn

 

[Onda]

Hi Jonn,

Here a very easy model of half pin - hole, using Linear gap in Cylindrical coordinate system (2D model).

It's just an example to how to run linar gap.
I've used the Patran Application : "Linear Gap" to set up the model.

hope it help!

Onda

 

[janipk]

Hi to everyone,

Thank you very very much Onda for your help!

I have done every thing like in given bdf file and now an example model is working but my actaul model( Fuselage part of A350) with 455699 dof is sitll not working. In reality I have a gap of 3.5 mm between two shells,even I have tried with a smaller gap of 0.15 mm also.

What could be the possible reasons?

Does anyone has some other suggestion?

waiting for your valueable suggestions!

Thanks,

Jonn

 

[Onda]

You could try to run (for debugging only) with PARAM BAILOUT -1 to see if a part of your model isn't well constrained.
It's the most common problem with linear gap.

Onda

 

[einsteinscz]

hi noda and janke

i have got into trouble like janke ,my model has about 60,000 dof. and i make linear gap element in axial direction for every contact parts ,using rb2 in Fy~Mz for other direction(i want to simulate flanges contact).
unfortunately. I just obtain a fatal message 'fatal message 1012'. I have tried my best doing.
So ,i want to know whether my model is huge for using linear gap element or i made mistakes in it.
i am waiting for experts answers
tks

 

[einsteinscz]

hi everyone

i have got into trouble with linear gap element
My model like flange contact have 500000 dof. i use linear gap method in axial direction and rbe2(Fy~Mz) in other direction.
unfurtunately, i just obtain some fatal message "fatal message 1012" no matter what i do. (try to change buffsize)
or wirte down "nastran system(1015)=1"
i want to know whether my model is huge for this method
or i have made mistakes?
thanks

 

[Onda]

I've run linear gap problems with more then 60,000 DOF.
I think that You have some problem in your model.

Onda