solid 3d, load test

[abyss84]

Hello everyone, I wrote an ansys program of a thermosiphon door hook, but unfortunately I found problems, related to the final part, that is to the plotting of the results, that is at this point the program gives me error:
visualization of the results of interest

/posts

pldisp,1!show the structure and its deformed

!plnsol,s,eqv!mostro chart and tension table

! I don't understand why, can you help me? I attach the program that I wrote, in two different ways, tell me according to you where I'm wrong, the piece is in normal iron430 cylindrical form.

I also carry the error that gives me when I try to launch the commands after the last /post1, i.e. those related to the plnsol etc...

perhaps mistaken in the definition of the ''et,1,187'' ? or in ''et,2,21'' ?

thanks in advance for the answers

 

[abyss84]

the mistake that gives me is:

'''the degree of freedom solution is not available. the pldisp command is ignored''''

 

[abyss84]

even because if it is not mistaken et,1,187 is based on the fact that the element 1 is composed in solid 187 with axes and ux,uy,uz movements.

 

[stefano.garbin]

pldisp does not plot anything because your analysis fails.
if you look at the output well gives you an error message "degrees of freedom exceeeded", which means that your model is not properly bound.

 

[stefano.garbin]

rectifying, there are a lot of things that don't fit in the input file.
Now I prepare a detailed answer.

 

[abyss84]

for the constraints I tried to create a master node and then apply the constraint all, since it is stuck to the wall, or directly applying constraints without the master node, but in both cases it does not work.. I don't understand where I was wrong.

 

[stefano.garbin]

finish
_

Construction of geometry

/prep7

I create the base area


k,1,0,0,0!creo 5 points, one in the center acts as center of circumference and 4 for cardinal points
k,2,0,0.004,0
k,3,0,0.004
k,4,0,-0.004,0
k,5,0,-0.004

larc,2,3,1,0.004!creo four curves that define the circumference
larc,3,4,1,0.004
larc,4,5,1,0.004
larc,5,2,1,0.004

al,1,2,3,4 !evidenzio the area contained between the 4 arc elements

!extrude the base area

voffst,1,0.05!Extrusion method of the area, for the following direction
The rule of the right hand

k,10,0.062,-0.008,0!creates also 4 kp on the other end 6,7,8,9
k,11,0.05,-0.00725,0
k,12,0.05,-0.00725,-0.02

!

vrotat,2,,,, 11,12,43.6!area 2 with kp 11 and 12 defining rotation


k,17,0.055,-0.002,0! center area 11
k,18,0.08,-0.012,0 average reverse arc point
k,19,0.105,-0.002,0 final point reverse arc
k,20,0.08,0.02425,0! reverse arc line rotation point

larc,17,18,20,0.03625! first line arc reverse
larc,18,19,20,0.03625! second line arc reverse

vdrag,11,,,,21,22 extrusion along reverse arc lines

ok, you are building a "extruded" geometry with diameter 2*0.004=0.008
What unit do you have in mind to use? Meters or millimeters? Further down you will define the characteristics of the material by putting e=210000 mpa!
so you have designed a thing with diameter of 8 microns!!! !

lesize,9,,40!I divide the first part
lesize,10,,40
lesize,11,,40
lesize,12,,40

lesize,17,,20!I divide the second curve
lesize,18,20
lesize,19,20
lesize,20,,20

lesize,24,,40!I divide the third part
lesize,25,40
lesize,27,,40
lesize,29,,40

lesize,32,,40!I divide the fourth curve
lesize,33,40
lesize,35,,40
lesize,37,,40

lesize,1,20,I divide the first circumference
lesize,2,,20
lesize,3,,20
lesize,4,,20

lesize,all,10

forget all sizing lines for the moment. Let me make ansys other generates an unnecessarily detailed model.

r,1.5e-3!real coasters for solid

et,1,187!definition of solid 187 elements
et,2,21!21 mass to apply force

Other comments:
1-What should this real constant serve? I don't understand!
2-as element type uses solid186, then you understand why.
You don't need mass21, take it out.

mp,ex,1,2.1e5 !proprieted material mpa
mp,nuxy,1,0.3
mp,dens,1,7850 !kg/m3

eye, elastic module in mpa (n/mm^2) and density in kg/m^3 are inconsistent.

type,1
real,1
mat,1

vmesh,all			!effettuo la meshatura

try to generate mesh with vsweep,all and you will see that it is all another thing.
vsweep generates an extruded mesh: less elements, faster and more precise solution. is not applicable to solid187 because it is a tetraheric element while solid186 is a "brick".

! generation of the rigid zone where to apply the load

n,10000000,0.08,-0.012,0!creo the knot to be bound to the hook

type,2
real,1
e,10000000
alls

Togli questa roba qui sopra

nsel,s,loc,x,0.0799,0.0801!select a set of knots included in an area
nsel,r,loc,y,-0.016,-0.008!s=select a new set
!r=reselect the previous set

nsel,a,,10000000

cerig,10000000,all,all!lego to the master node 10000000 selected slave nodes

♪

before making the cerig I also selected the additional node

! generation of the rigid zone where to apply constraints


!

nsel,s,loc,y-0.00001,0.00002
♪
nsel,r,loc,z,-0.004,0.004!vincolo the base of the hook

d,all,all
♪

f,10000000,fy,-30000!

end

who sows me ok.

! %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

! resolution of the generated model

In the solutor
/solu

Model resolution
The

save

finish



! %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

visualization of the results of interest

/posts

pldisp,1!show the structure and its deformed

!plnsol,s,eqv!mostro chart and tension table

!

then see how to fix the size of the hook and the properties of the material and see how it turns ok?

 

[abyss84]

I now submit all the amendments....just made the positive or negative result thank you very much for the immense help

 

[abyss84]

what real constants are useful according to you to insert with ''r,1,...''?

 

[abyss84]

I made all the changes you told me, or at least I think.

I changed from 2.1e5 to 2.1e11, so I work in meters.

now the program comes to the end, but from two mistakes, indeed two warnings, which are:

1 - label rotz is not an active degree of freedom. the cerig command is ignored.

2 - I don't know if it's a mistake anymore.

and of course I plot everything, but as if there were no loads applied, how can I solve?

 

[stefano.garbin]

see the attached file.
I fixed two or three things and allowed myself to replace the cerig command with rbe3.
using rbe3 I had to re-introduce the mass21 because it is required.

 

[abyss84]

Thankseeee... now it's perfect... you did well to put the changes, you made me understand very well all the steps...I wanted to ask you another thing...I also wrote this other program, of a plate, in 2d, always in fe430 that I from warnings...well 4 and I don't understand why.

Another thing, do you think it's okay here with the ''lesize'?

 

[stefano.garbin]

What warning are they? Please post precise and circumstantial questions, I don't always have time to take your input files and verify them.
You can't think there's someone doing your job.

 

[abyss84]

you are fully right, warnings are the following, placed them in an image, so you also see the depicted plate.

use:

- definition of the type of element: et,1,43
- mp,ex,1,2.1e11!
- mp,dens,1,7850! material density
- type,1
- real,1
- Mat,1
- amesh,all

- introduction of the mass type element
et,2,21
type,2

 

[stefano.garbin]

warning that you have to worry is that both elements 43 and 21 use the same real constant. Wrong.
you must create a real constant also for the mass21.

et,2,21
r,2,massa
type,2
real,2

uses the shell181 instead of 43 because it became "undocumented".
for the "shape warning" modifies the mesh so you have elements that vary more gently and smoothly in size.

 

[abyss84]

I made the following changes:

et,2,21
r,2,1,1,1
type,2
real,2

I also added, ''mp,nuxy,1,0.3' because it required me the shell181.

What do you mean by sweeter mash? How can I make it? I used ''amash' as a command for meshare

 

[stefano.garbin]

search the mopt command, you will find a lot of very useful options.

 

[abyss84]

I'm trying the command you gave me with options, like

mopt,vmesh,alternate or mopt,qmesh,default but nothing happens to me, possibly I leave the basic one that is amesh.

However there are a thousand options I didn't know exactly.

last thing and then I stop to assillate you, applying the load to the plate, I have two main forces, an orthogonal on the plane of the plate called va=4461n and a ma=6221nm that I stick to the central node. How can I write them on ansys?

I thought:

f,999999,mx,6221, for the moment but

and

f,999999,fz,4461

because the top of the plate is xy.

Could you go? or to introduce another written command?