apdl [soln's options]

[volaff]

Hey, everybody.

after many vicissitudes I corrected the panel model that contains the hp.

I removed the constraints and loads and then corrected geometry by remeshating the various areas affected by the change.

When, though, I go to do static analysis, the message appears to me:

"" a small equation solver pivot term has been encountered at the uy
degree of freedom of node 38941. ansys has automatically constrained
This degree of freedom. check for an insufficiently constrained
model.
"

if I solve in scattered mode, a similar error if I solve pcg.

as they suggested this error could be due to parts of the model not properly bound for which they urged me to carry out a modal analysis to verify the possible presence of part of the rigid body not bound.

I point out that in my model it was not defined the density for which I inserted a similar to that of steel.

I realized the modal analysis with the following options:


sopt: block lanczos

No. od modes to extract:10

no. of modes to expand: 10

it's been three hours and the analysis is less than half, at cycle number 6.

My pc has 6 gb of ram.

I was wondering if the procedure was correct even in relation to the times.

Thank you all.

I have done this

 

[volaff]

incomplete message: I have done this analysis but the pc seems planned.

Moreover, if possible, I wanted to ask if there is a command that allows to understand, knowing the node, which is the area to which it belongs. I feel like there's mesh problems.

thanks to all

 

[stefano.garbin]

so you see the node that gives you warning.
attention, the fact that this warning has appeared does not necessarily imply that the simulation is wrong.

nodenum=38941

*get,minx,node,,mnloc,x, , , ,
*get,miny,node,,mnloc,y, , , ,
*get,minz,node,,,mnloc,z, , , ,

*get,maxx,node,,mxloc,x, , , ,
*get,maxy,node,,mxloc,y, , , ,
*get,maxz,node,,mxloc,z, , , ,

bbx=abs(maxx-minx)
bby=abs(maxy-miny)
bbz=abs(maxz-minz)

diag=(bbx**2+bby**2+bbz**2)**0.5

px=nx(nodenum)
py=ny(nodenum)
pz=nz(nodenum)
px1=px-diag/10
py1=py-diag/10
pz1=pz-diag/10
/an3d,arrow,10,px1,py1,pz1,px,py,pz

 

[volaff]

Thank you very much for the answer.
cmq this is not a warning but a mistake.

the problem is that I wanted to understand to which area the "incrimined" node belonged so as to make the right considerations.

I'm also trying the modal analysis but it's very slow and ansys crashes all the time.

Remember how you can do to allocate more rams for analysis? ?

bscoption but I don't know what to insert into the next parameters.
my notebook has 6 gb of ram

Thank you very much for the tip.
Good job!

ps: In this way I highlighted the area of belonging to that ef node, effectively, is an area that I remeshato after cleaning it.

Maybe I try to remake the mesh of that area (which I already did for all areas) and see if I can pull out something good.

Thanks again

 

[volaff]

hi, I realized that some nodes having different numbering share the same position and this,sec me, causes the non-good achievement of the analysis.

For example, I noticed that:
node x y z thxy thyz thzx
38941 50.000 151.64 3.7000 0.00 0.00 0.00

node x y z thxy thyz thzx
265357 50.000 151.64 3.7000 0.00 0.00 0.00


I wondered if there was a way to highlight the double knots (that is, they have the same position) and possibly join them so as to create a single knot.

the second question can be resolved with the nummrg command, but the first I have no idea how to solve it if not with the nlist command.

Thank you very much.

"if in the model there are pairs of distinct knots (different number) that have the same coordinates, the elements connected to such knots are treated as disjoining each other (as if in the model there was a fracture or a continuity solution)"

taken from an online pantry.

I think that's my problem.

Thanks again

 

[volaff]

Hi. I solved the problem by applying to all knots the nummrg command and analysis went well: the results are disappointing so I have to review some things for sure.

Thank you all.
Good Sunday.

 

[volaff]

ps: small grinding.
by applying the nummrg command I also take nodes that "I don't care": I must by force select the knots having the same coordinates to solve the problem.

a soluzioen could be to launch every time an analysis so in the error message pull out, from time to time, a "incriminate" knot but surely there will be a faster and painless solution.

Hopefully.
I wish a dark Sunday to all!

 

[stefano.garbin]

nummrg joins the knots that are closer than a certain tolerance.
example:
nummrg,node,1e-3
unites the nearest knots of 1e-3

If you want me to work only on the selected nodes and not on the whole model write like this:
nummrg,node,1e-3,sele

 

[volaff]

Thank you very much stefano.
I finally realized that the problem was due to incorrect creation of beam4 elements by me in the new model.

then a problem has arisen in the creation of beam4 elements of the cleaned areas that in the original model were of the type:

elem mat typ rel esy sec nodes

192719 5 4 3 100 2 36990 60696 0
192720 5 4 3 100 2 37400 60697 0
192721 5 4 3 100 2 37401 60698 0
192722 5 4 3 100 2 37002 60699 0

while in the modified model were:

elem mat typ rel esy sec nodes

302561 5 3 3 100 23 270487
302562 5 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 3 2 3 2 3 2 3 3 3 2 3 2 3 2 3 3 2 3 2 3 2 3 2 2 3 2 3 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2
302563 5 4 3 100 23 270462 271205 0
302564 5 4 3 100 23 270461 271204

in practice it gave me (for a part of the beam4) same mat, same real, same esys but different section.


thanks to the friends of the forum I solved by importing the following line of code:

♪
*do,i,1,416
!
!
!
!
*get,n2,node,nxtl
type,4
mat,5
secn,2
real,3
esys,100
e,node(kx(4999+i),ky(4999+i),kz(4999+i), node(kx(7999+i),ky(7999+i),kz(7999+i))
*end

Maybe someone has the same problem.

I have only a small doubt: They told me that real constant should not be in conflict with the section, but in what sense? !

now the model seems to go even if it is definitely improved.
Thank you all.
Have a good day.

 

[volaff]

hi to everyone, I realized that the code above (which I understood well or bad) gives me a kind of anomaly.

as you can see from the figure the beam4 elements are actually created but not all (some knot is "high").

I made up with this other piece of code:
"finish
/prep7

♪
*do,i,1,416
ksel,s,,7999+i
Ksel,a,,4999+i
♪
*get,n1,node,nxth
*get,n2,node,nxtl
type,4
mat,5
secn,2
real,3
esys,100
e,n1.n2
*end

"

but now it sogees the ark.
I realized that on the original model between the nodes I modified (actual hp) there are type1 elements that I cannot understand the "functional".

But if I don't put them, the analysis leads to completely high results.

now I wanted to insert them into the modified model to make a simple comparison between the duies models.

Then it will be my concern to fire me from the prof if those shell elements are to be positioned there: I have a half idea why they are there, but I want to be sure (I think they have the hp).

In practice I would like to create that quadrangular element (figure 1 and 2), of which the extremes are known hp (and, therefore, nodes) .

I tried but an error appears:

_
quadrilateral element 291224 has a zero or negative determinant of the
jacobian matrix at one of its sampling locations.

_
the e command cannot store element 291224, because of an element shape
error.


thanks to all
Good evening

 

[volaff]

edit: problem solved.
just put the knots (hp) in the right sequence (clockwise or anti-clockwise) and on creating strange interweathers.
And yet I was convinced that I did the thing in a correct sequence, but rechecking. .

Good weekend, everyone!