[XANSYS] [WB] [APDL] Weld size using cpintf | High forces on midside nodes
Hi Xansers,
I am trying to find the weld stresses (weld shear and weld tension) using the forces output in 3 -directions (Fx, Fy and Fz) using FSUM/PRNLD command in Ansys post-processing with APDL.
The mesh (SHELL281, 8 noded quadratic elements) is uniform in size (=10mm) across the model and the weld is simulated using "CPINTF" command in Ansys. So, two set of nodes of the model where there is a weld are connected through couplings (one by one in a loop).
During postprocessing, I am selecting one node set from a weld (couplings between two set of nodes) and after each node selection, I write the forces Fx, Fy and Fz in a text file. I know the spacing between nodes so for each node I get Fx, Fy and Fz and I calculate the resultant force causing shear (two directions) and I do a SRSS of forces Fx, Fy and Fz (square root of sum of squares) - which gives shear force per unit element length (distance between two nodes) using the former and unit force (SRSS) per unit element length using the latter.
I then pick a size of weld and calculate throat, then dividing this shear force per unit length of element by the throat which gives me the shear stress and same for the unit stress (SRSS of Fx Fy and Fz per unit element length per throat). Then compare these values with allowable as min.[0.4Sy (base material),0.3Su] (outlined in AWS D1.1 table 2.3)
Problem is that I have a mid-side node and it connects two elements whereas the corner nodes connects 4 elements. And when I calculate the weld stress using a full penetration weld (size equals to plate thickness) the weld fails. There is high force on one of the midside nodes. I do not understand why it happens and what can I do to avoid this high force. If I exclude that node, then I need a less size of weld (15mm plate thk will require 8mm groove weld) and all is hunky-dory.
Shall I mesh with linear elements and see the forces so that I only have corner nodes to get the Fx, Fy and Fz for these nodes?
FYI, the coupling or cpintf command generates coupling between midside nodes also (in WB) which I can see in Ansys Classic if I save the db and rst file in WB and then open the same in Ansys Classic.
Best regards,
Shiraz Khan
Senior Engineer
Topsoe
There is option to select only edge nodes
check help manual will get
Use fir selecting edge nodes
NSEL,,EDGE something like this
Regards
Paramesh
On Tue, 16 Jan, 2024, 11:16 am Shiraz Khan [KHSH] via Xansys, <
xansys-temp@list.xansys.org> wrote:
Hi Xansers,
I am trying to find the weld stresses (weld shear and weld tension) using
the forces output in 3 -directions (Fx, Fy and Fz) using FSUM/PRNLD command
in Ansys post-processing with APDL.
The mesh (SHELL281, 8 noded quadratic elements) is uniform in size (=10mm)
across the model and the weld is simulated using "CPINTF" command in Ansys.
So, two set of nodes of the model where there is a weld are connected
through couplings (one by one in a loop).
During postprocessing, I am selecting one node set from a weld (couplings
between two set of nodes) and after each node selection, I write the forces
Fx, Fy and Fz in a text file. I know the spacing between nodes so for each
node I get Fx, Fy and Fz and I calculate the resultant force causing shear
(two directions) and I do a SRSS of forces Fx, Fy and Fz (square root of
sum of squares) - which gives shear force per unit element length (distance
between two nodes) using the former and unit force (SRSS) per unit element
length using the latter.
I then pick a size of weld and calculate throat, then dividing this shear
force per unit length of element by the throat which gives me the shear
stress and same for the unit stress (SRSS of Fx Fy and Fz per unit element
length per throat). Then compare these values with allowable as min.[0.4Sy
(base material),0.3Su] (outlined in AWS D1.1 table 2.3)
Problem is that I have a mid-side node and it connects two elements
whereas the corner nodes connects 4 elements. And when I calculate the weld
stress using a full penetration weld (size equals to plate thickness) the
weld fails. There is high force on one of the midside nodes. I do not
understand why it happens and what can I do to avoid this high force. If I
exclude that node, then I need a less size of weld (15mm plate thk will
require 8mm groove weld) and all is hunky-dory.
Shall I mesh with linear elements and see the forces so that I only have
corner nodes to get the Fx, Fy and Fz for these nodes?
FYI, the coupling or cpintf command generates coupling between midside
nodes also (in WB) which I can see in Ansys Classic if I save the db and
rst file in WB and then open the same in Ansys Classic.
Best regards,
Shiraz Khan
Senior Engineer
Topsoe
Xansys mailing list -- xansys-temp@list.xansys.org
To unsubscribe send an email to xansys-temp-leave@list.xansys.org
If you are receiving too many emails from XANSYS please consider changing
account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Hi Shiraz,
With srss after recombination the nodal forces are not written to the file.
Consequently, it may give a wrong result.
Try using presol,f which takes into account the forces at the nodes at the
weld for each element at the interface. Forces are written to element db.
Thanks,
Nelson
On Mon, Jan 15, 2024 at 9:46 PM Shiraz Khan [KHSH] via Xansys <
xansys-temp@list.xansys.org> wrote:
Hi Xansers,
I am trying to find the weld stresses (weld shear and weld tension) using
the forces output in 3 -directions (Fx, Fy and Fz) using FSUM/PRNLD command
in Ansys post-processing with APDL.
The mesh (SHELL281, 8 noded quadratic elements) is uniform in size (=10mm)
across the model and the weld is simulated using "CPINTF" command in Ansys.
So, two set of nodes of the model where there is a weld are connected
through couplings (one by one in a loop).
During postprocessing, I am selecting one node set from a weld (couplings
between two set of nodes) and after each node selection, I write the forces
Fx, Fy and Fz in a text file. I know the spacing between nodes so for each
node I get Fx, Fy and Fz and I calculate the resultant force causing shear
(two directions) and I do a SRSS of forces Fx, Fy and Fz (square root of
sum of squares) - which gives shear force per unit element length (distance
between two nodes) using the former and unit force (SRSS) per unit element
length using the latter.
I then pick a size of weld and calculate throat, then dividing this shear
force per unit length of element by the throat which gives me the shear
stress and same for the unit stress (SRSS of Fx Fy and Fz per unit element
length per throat). Then compare these values with allowable as min.[0.4Sy
(base material),0.3Su] (outlined in AWS D1.1 table 2.3)
Problem is that I have a mid-side node and it connects two elements
whereas the corner nodes connects 4 elements. And when I calculate the weld
stress using a full penetration weld (size equals to plate thickness) the
weld fails. There is high force on one of the midside nodes. I do not
understand why it happens and what can I do to avoid this high force. If I
exclude that node, then I need a less size of weld (15mm plate thk will
require 8mm groove weld) and all is hunky-dory.
Shall I mesh with linear elements and see the forces so that I only have
corner nodes to get the Fx, Fy and Fz for these nodes?
FYI, the coupling or cpintf command generates coupling between midside
nodes also (in WB) which I can see in Ansys Classic if I save the db and
rst file in WB and then open the same in Ansys Classic.
Best regards,
Shiraz Khan
Senior Engineer
Topsoe
Xansys mailing list -- xansys-temp@list.xansys.org
To unsubscribe send an email to xansys-temp-leave@list.xansys.org
If you are receiving too many emails from XANSYS please consider changing
account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to
xansys-mod@tynecomp.co.uk and not to the list
Its not clear to me if you are doing the following, but I think its necessary to get good results. First, you need to select only elements on one part. Then select only nodes on that part that are on the weld. Next, perform an FSUM,RSYS. this should give you accurate weld reactions. Second, it does not appear that you are considering moments in the weld group. You will get these from the FSUM command, but to be accurate, you must place a local coordinate system at the centroid of the weld group, get the global coordinates of the origin of that csys (*get,xx,cdsy,actsys,loc,x, etc) and set that location as the summation point (spoint,,xx,yy,zz). Hope this helps.
Shiraz,
Rick Fischer brought up some important points. Be sure to consider his suggestions.
Also, be aware that quadratic elements have differing stiffness at the corner nodes vs the midside nodes. This is due to the quadratic functions used for displacement interpolation within the element. As a consequence, interpreting the nodal forces (and reaction forces) for quadratic elements can be somewhat complicated. I suspect this is why you are seeing higher forces on the midside nodes relative to the adjacent corner nodes.
Read the theory manual for SHELL281, as well as the section explaining quadratic elements and their shape functions. Then, create a very simple problem involving only a couple elements, connected via coupling, with a simple straight forward load(s), and review the nodal forces so you can understand how these elements work.
--
Mitch Voehl
CEO and Engineering Consultant
Summit Analysis, Inc.
78748 410th Ave
Lakefield, MN 56150
Specializing in the use of ANSYS (R) finite element analysis software
On 01/15/2024 11:44 PM CST Shiraz Khan [KHSH] via Xansys xansys-temp@list.xansys.org wrote:
Hi Xansers,
I am trying to find the weld stresses (weld shear and weld tension) using the forces output in 3 -directions (Fx, Fy and Fz) using FSUM/PRNLD command in Ansys post-processing with APDL.
The mesh (SHELL281, 8 noded quadratic elements) is uniform in size (=10mm) across the model and the weld is simulated using "CPINTF" command in Ansys. So, two set of nodes of the model where there is a weld are connected through couplings (one by one in a loop).
During postprocessing, I am selecting one node set from a weld (couplings between two set of nodes) and after each node selection, I write the forces Fx, Fy and Fz in a text file. I know the spacing between nodes so for each node I get Fx, Fy and Fz and I calculate the resultant force causing shear (two directions) and I do a SRSS of forces Fx, Fy and Fz (square root of sum of squares) - which gives shear force per unit element length (distance between two nodes) using the former and unit force (SRSS) per unit element length using the latter.
I then pick a size of weld and calculate throat, then dividing this shear force per unit length of element by the throat which gives me the shear stress and same for the unit stress (SRSS of Fx Fy and Fz per unit element length per throat). Then compare these values with allowable as min.[0.4Sy (base material),0.3Su] (outlined in AWS D1.1 table 2.3)
Problem is that I have a mid-side node and it connects two elements whereas the corner nodes connects 4 elements. And when I calculate the weld stress using a full penetration weld (size equals to plate thickness) the weld fails. There is high force on one of the midside nodes. I do not understand why it happens and what can I do to avoid this high force. If I exclude that node, then I need a less size of weld (15mm plate thk will require 8mm groove weld) and all is hunky-dory.
Shall I mesh with linear elements and see the forces so that I only have corner nodes to get the Fx, Fy and Fz for these nodes?
FYI, the coupling or cpintf command generates coupling between midside nodes also (in WB) which I can see in Ansys Classic if I save the db and rst file in WB and then open the same in Ansys Classic.
Best regards,
Shiraz Khan
Senior Engineer
Topsoe
Xansys mailing list -- xansys-temp@list.xansys.org
To unsubscribe send an email to xansys-temp-leave@list.xansys.org
If you are receiving too many emails from XANSYS please consider changing account settings to Digest mode which will send a single email per day.
Please send administrative requests such as deletion from XANSYS to xansys-mod@tynecomp.co.uk and not to the list