Ansys APDL Mesh

[Amine A]

Hello ,
anyone knows how to do such a much in a circle (2D plane strain) on APDL please ?

 

[petb]

Create a circle, then a rectangle and use boolean operations to subtract the rectangle from the circle. Use LESIZE to set the number of line divisions and then use AMAP to map mesh the areas.

/PB

 

[Amine A]

it doesn't work look,

and I have a question , normally it won't be considered as a circle if I do like what you said ,no ? it will be considered as a cricle that contains hole

 

[petb]

Look, you got a few tips on what command to use to do some geometry modelling. The documentation is really good and the few tips I gave you should have been enough to get you started. Below is some APDL-code to generate a model similar to yours. Step through the commands line by line so you will understand what is happening. [pre]/prep7
ET,2,MESH200
KEYOPT,2,1,6
KEYOPT,2,2,0
/pnum,kp,1
/pnum,line,1
/pnum,area,1
/PSYMB,LDIV,1
csys,1
k,10,.5,0
*repeat,4,1,,90
k,20,1,0
*repeat,4,1,,90
/replot
gplot
l,20,21
l,21,22
l,22,23
l,23,20
/replot
csys,0
l,10,20
*repeat,4,1,1
l,10,11
l,11,12
l,12,13
l,13,10
/replot

al,1,6,9,5
*repeat,3,1,1,1,1
al,5,12,8,4
a,10,11,12,13
gplot

lsel,s,,,1,4
lsel,a,,,9,12
lesi,all,,,12
lsel,inve
lesi,all,,,5
lsel,all
lplot

amap,4,13,23,20,10
amap,5,10,11,12,13
amap,1,10,20,21,11
*repeat,3,1,1,1,1,1[/pre]

BTW, creating a line between two KPs in a cylindrical csys will create an arc.

 

[rickfischer51]

Way too complicated. Try this:

/prep7
pcirc,1
rectng,-.25,.25,-.25,.25
asba,1,2,,delete,delete
ssln,,.5
allsel
lesize,all,.1
et,1,183
esize,.2
amesh,all

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[Amine A]

Thanks you so much , the first code of Mr petb works good, but can you please tell me how to do that without coding (I will try to understand the code later), just steps with that modelling window , because I'm new user of this software

 

[rickfischer51]

Look up each command in the documentation. Scroll to the bottom of the page. Last item is Menu Paths. That will show you how to access the command from the GUI.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[Amine A]

it works ! thank youu !

 

[Amine A]

Can you tell me please how to plot kinetic , elastic strain and total energies ??

 

[Amine A]

and what's the difference between defining loads in "prepocessor" and defining loads in "solution" ?

 

[petb]

To plot results you use PLNSOL for nodal solution quantities and PLESOL for elemental results. Both are very well documented in the help ( Mechanical APDL Command Reference). For each of them, all available items are listed in the respective command reference page. The items available to plot in your indiviual case depends on your choice of analysis type, element type and output controls (what items you've told Ansys to put in you results database)

There is no difference in defining loads in /prep7 or in /solu.

 

[Amine A]

Ok I will see thanks ! when I change the mesh just with a different one ( wether with bigger elements or smaller) , and define again exactly the same loads it doesn't give me same results , and material change even it s behaviour , it penetrates in the rigid body ! why this happens