RIGID BODY CHECKS IN 4, 5 and 6 DIRECTIONS FAIL 2

[HawksOkeyoJr]

Hallo guys,

I am not newbie in NASTRAN environment, but I don't seem to crack what on earth is wrong with my model (Model Attached).
I ran a FREE-FREE check on my structure and requested for all the 'SETS', to my surprise, the model fails the 4, 5 and 6 directions while the eigenfrequencies show that the structure is fully a rigid one. Can somebody with more experience help me crack it please!. I will really be grateful for your effort. Thanks in advance.

*** USER INFORMATION MESSAGE 7570 (GPWG1D)
RESULTS OF RIGID BODY CHECKS OF MATRIX KGG (G-SET) FOLLOW:
PRINT RESULTS IN ALL SIX DIRECTIONS AGAINST THE LIMIT OF 1.232662E-04
DIRECTION STRAIN ENERGY PASS/FAIL
--------- ------------- ---------
1 1.898201E-09 PASS
2 1.770204E-09 PASS
3 1.048686E-09 PASS
4 1.633240E-03 FAIL
5 1.100441E+01 FAIL
6 4.751907E+00 FAIL

MODE EXTRACTION EIGENVALUE
NO. ORDER
1 1 -9.614290E-06
2 2 -3.726920E-06
3 3 -1.669621E-06
4 4 -4.575413E-07
5 5 4.400790E-07
6 6 3.495363E-06
7 7 4.155432E+02
8 8 5.656006E+02
9 9 8.297285E+03
10 10 1.224819E+04

 

[Naffoussi]

Hi,

First of all, your unit system is incoherent...you are working in mm, so start by changing:

E = 73000 to 73e+6MPa
Density = 2.7e-9!!? to 2.7e-4 g/mm3







Seif Eddine Naffoussi, Stress Engineer

http://www.Innovamech.com

33650 Martillac û France

 

[rb1957]

i couldn't see any constraints ?

another day in paradise, or is paradise one day closer ?

 

[Naffoussi]

@rb1957
he don't need a constraint for a free free analysis nor for ground check.

Seif Eddine Naffoussi, Stress Engineer

http://www.Innovamech.com

33650 Martillac û France

 

[HawksOkeyoJr]

@ CompositeCurves
Nothing is wrong with the units,
E= 73100 Nmm-2
Density = 2.78E-9 Tonmm-3

So, it can't be the units.

@ rb1957, as CompositeCurves specified, we don't need constrains for a fee-free check.

 

[Naffoussi]

Sorry about the units , you are right.

Seif Eddine Naffoussi, Stress Engineer

http://www.Innovamech.com

33650 Martillac û France

 

[HawksOkeyoJr]

@ CompositeCurves
If you have time and found out something, just let me know. Thanks for taking your time.
I am also working on it, in case my solution works, I will post it.

 

[rb1957]

so maybe the check is telling you you have a mechanism, like an elbow joint ?

units ... yes, not the problem but are Tonnes the consistent mass unit (or weight unit) for N ?

another day in paradise, or is paradise one day closer ?

 

[Naffoussi]

Did you try to connect your RBE2 to multiple slave nodes instead of node to node?
Regarding the geometry and connection between parts I will be curious to see what it gives...

Seif Eddine Naffoussi, Stress Engineer

http://www.Innovamech.com

33650 Martillac û France

 

[HawksOkeyoJr]

@ rb1957, tonnes are mass units. The units have no problem. I don't get the question with the elbow joint..... Do you mean it might be rotating from that point??

@ CompositeCurves, Adding more slaves is what I thought would solve the issue, I just did that, but the results stay the same.... Still FAILS.

 

[stressebookllc]

This is what I got:

MODAL_FIXED SUBCASE 1

R I G I D - B O D Y E I G E N V A L U E S

MODE EIGENVALUE STRAIN ENERGY
NUMBER EXTRACTED NORMALIZED EXTRACTED NORMALIZED
1 1.588782E-10 3.581042E-13 3.669735E-07 8.271415E-10
2 3.167704E-10 7.139860E-13 8.286201E-07 1.867672E-09
3 7.115370E-10 1.603772E-12 1.778880E-06 4.009514E-09
4 8.235215E-10 1.856180E-12 8.218623E-07 1.852440E-09
5 1.061114E-09 2.391703E-12 2.890820E-06 6.515777E-09
6 2.582696E-09 5.821279E-12 3.670704E-06 8.273599E-09

All I did was remove param bailout, remove autospc and used neinastran.

http://www.stressebook.com

Stressing Stresslessly!

 

[HawksOkeyoJr]

@ stressebookllc , thats for taking your time, I do appreciate it and i can see you have very good values for the modes, but the thing is, I am using MD Nastran and those PARAMs are mandatory for the model to be accepted.
I guess i will never get around it, BUT am still trying......Thanks for taking your time...If you have a shot at it again, just let me know.

 

[rb1957]

who is telling you you have to use param bailout ? you is telling you you must use autospc ?? these are both potentially very dangerous options (particularly bailout) as they "fix" model problems without telling you.

looking at your structure, see attmt, i think you've got a pattern of rivets where i've drawn boxes, but i think you've only got a line of rivets where i've drawn lines ... if so, then the lines will create a mechanism.

another day in paradise, or is paradise one day closer ?

 

[HawksOkeyoJr]

@ rb1957. Hallo Sir, thank you for your time.... What i meant by "Those PARAMs" are mandatory, was that: BAILOUT and AUTOSPC MUST be "NO". Our friend Stressebookllc removed AUTOSPC and when its absent, its taken as default which is "YES" and that "YES" is what we are trying to avoid.

All in all, coming back to your suggestion, I think you are right, Some mechanism exists in the structure...The positions you indicated are the ones with fasteners (All the RBEs on the model, indicate the positions of the FASTENER). I guess, i will have to give up on it. The rest of the checks are perfectly correct and results generated from GLOADs, are perfectly acceptable.

 

[rb1957]

your structure looks full of very flexible loadpaths ... not a criticism. whilst the results look ok, the problem could remain with low frequency modes, whihc (if this is for auto) could be a problem. you can improve the design by removing the single line attmts so the structure is more rigid.

another day in paradise, or is paradise one day closer ?

 

[HawksOkeyoJr]

@rb1957, I welcome Criticism with open arm....)))). The structure is just a protection plate (to prevent us human from hanging on a pipe behind the structure) and I just needed to calculate the interface point loads.
I am not the designer, I am the stress guy and of course I will have to make suggestions on how to improve it and that's why am thankful for your "Experienced look". By the way, which single line attachment are you talking about (A screenshot would be great).
Thanks for your contribution.

 

[rb1957]

the fastening is very minimal ... any time you can see all the connections between different pieces being co-linear, this isn't good; it's not Bad but it does allow the structure to vibrate.

careful designing "covers" ... they have a nasty habit of vibrating and cracking, 'cause "they're only covers".

another day in paradise, or is paradise one day closer ?

 

[rb1957]

oh, and don't be scared of them there designers ! if you Need a change, it'll happen, if you Want a change i'd discuss with your lead/supervisor. what company experience can you draw on ?
"this is the way we're always done it, everyone likes it"
"this is new for us, but we (think we) know what we're doing"
"the job doesn't have budget to fuss it ... show it good, now get out (i've got real work to do)"
"jimmy down in manufacturing likes it so it's probably good"
...

another day in paradise, or is paradise one day closer ?

 

[HawksOkeyoJr]

@rb1957, Thanks for a great observation. The fastener really do look too co-linear. I will try to stagger some and see the outcome.
On your question, I am still young in the industry, we just fast learner, but we are getting there....)))))

 

[nlgyro]

to return back the OP question:

Such high grounding values in the rotational dof's usually occurs when the c.g of the model is far away from the origin of the basic co-ordinate system.

The c.g of your FEM is at [6.532052E+04,-1.616993E+02,-3.607411E+02]

When the grounding check is recomputed by using:

GROUNDCHECK(SET=ALL,GRID=10000,DATAREC=YES,RTHRESH=0.8)=YES ----> grid 10000 being an arbitrary grid I created at the model c.g, the g-set grounding results are

*** USER INFORMATION MESSAGE 7570 (GPWG1D)
RESULTS OF RIGID BODY CHECKS OF MATRIX KGG (G-SET) FOLLOW:
PRINT RESULTS IN ALL SIX DIRECTIONS AGAINST THE LIMIT OF 1.232662E-04
DIRECTION STRAIN ENERGY PASS/FAIL
--------- ------------- ---------
1 2.887553E-09 PASS
2 3.719610E-09 PASS
3 2.314525E-09 PASS
4 5.442943E-04 FAIL
5 1.249674E-03 FAIL
6 5.989947E-04 FAIL

SOME POSSIBLE REASONS MAY LEAD TO THE FAILURE:
1. CELASI ELEMENTS CONNECTING TO ONLY ONE GRID POINT;
2. CELASI ELEMENTS CONNECTING TO NON-COINCIDENT POINTS;
3. CELASI ELEMENTS CONNECTING TO NON-COLINEAR DOF;
4. IMPROPERLY DEFINED DMIG MATRICES;

On examining the ground forces at these d.o.f's which are failing:

DIRECTION 4
G R O U N D C H E C K F O R C E S ( G - S E T )

POINT ID. TYPE T1 T2 T3 R1 R2 R3
7467 G 0.0 -1.504304E-07 0.0 0.0 0.0 0.0
7666 G 0.0 1.250181E-07 0.0 0.0 0.0 0.0
7670 G 0.0 1.275758E-07 0.0 0.0 0.0 0.0
7683 G 0.0 1.210719E-07 0.0 0.0 0.0 0.0
1 MSC.NASTRAN JOB CREATED ON 26-SEP-14 AT 15:43:46 JANUARY 31, 2015 MD NASTRAN 5/ 9/08 PAGE 13

0
DIRECTION 5
G R O U N D C H E C K F O R C E S ( G - S E T )

POINT ID. TYPE T1 T2 T3 R1 R2 R3
3106 G 0.0 0.0 1.109781E-07 0.0 0.0 0.0
3127 G 0.0 0.0 -1.000477E-07 0.0 0.0 0.0
7645 G 0.0 0.0 -1.005828E-07 0.0 0.0 0.0
7811 G 0.0 0.0 1.154840E-07 0.0 0.0 0.0
7916 G -1.097471E-07 0.0 0.0 0.0 0.0 0.0
7953 G 0.0 0.0 1.028170E-07 0.0 0.0 0.0
7970 G 0.0 0.0 -1.192093E-07 0.0 0.0 0.0
7983 G 0.0 0.0 -1.192093E-07 0.0 0.0 0.0
7987 G -1.211877E-07 0.0 0.0 0.0 0.0 0.0
7990 G -1.066569E-07 0.0 0.0 0.0 0.0 0.0
1 MSC.NASTRAN JOB CREATED ON 26-SEP-14 AT 15:43:46 JANUARY 31, 2015 MD NASTRAN 5/ 9/08 PAGE 14

0
DIRECTION 6
G R O U N D C H E C K F O R C E S ( G - S E T )

POINT ID. TYPE T1 T2 T3 R1 R2 R3
7405 G 0.0 1.962926E-07 0.0 0.0 0.0 0.0
7437 G 0.0 -1.873332E-07 0.0 0.0 0.0 0.0
7586 G 0.0 -1.639128E-07 0.0 0.0 0.0 0.0
7597 G 0.0 1.937151E-07 0.0 0.0 0.0 0.0
7644 G 0.0 1.639128E-07 0.0 0.0 0.0 0.0
7666 G 0.0 -1.937151E-07 0.0 0.0 0.0 0.0
7670 G 0.0 -1.788139E-07 0.0 0.0 0.0 0.0
1 MSC.NASTRAN JOB CREATED ON 26-SEP-14 AT 15:43:46 JANUARY 31, 2015 MD NASTRAN 5/ 9/08 PAGE 15


The groundng forces are practically zero (< 1.e-6), so your modeling is just fine, and its not worth the effort and time to clean your model by chase after grounding forces in the order of 1.e-7 !!