Would an old fashioned prestress restart work for this case ?

Keith DiRienz, P.E.
FEA Technologies
Office: 949.910.7049

On 4/14/2025 7:20 AM, Bohlen, Dan (GE Aerospace, US) via Xansys wrote:

--

Keith DiRienz, P.E.
FEA Technologies
Office: 949.910.7049

Well, without saying TOO much.  I have a part at rest, but there are some residual strains baked into the part due to manufacturing.  Our supplier gives us a set of plastic strains we apply to the model and then we do our standard analysis.

I found some examples in the verification manual.  I think my biggest issue now is I'm not sure how to translate what we get from the supplier to the NISTATE command.  I tried a 1 element model and it would converge when I put the strains on the way I thought they should go.

Hoping to get a PhD engineering mechanics guy here to look at it.  I'm not even sure how you put plastic strains on a model - wouldn't it have to be elastic+plastic strains?  Our in house program may take that into account.

Dan

-----Original Message-----
From: Keith DiRienz via Xansys xansys-temp@list.xansys.org
Sent: Monday, April 14, 2025 1:40 PM
To: xansys-temp@list.xansys.org
Cc: Keith DiRienz fea-technologies@cox.net
Subject: [Xansys] Re: playing with inistate Ansys 2024

Would an old fashioned prestress restart work for this case ?

Keith DiRienz, P.E.
FEA Technologies
Office: 949.910.7049

On 4/14/2025 7:20 AM, Bohlen, Dan (GE Aerospace, US) via Xansys wrote:

--

Keith DiRienz, P.E.
FEA Technologies
Office: 949.910.7049

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

Dan
Not sure if it helps but you can do this directly in WB very easily.  Connect the Solution to the model sections of two systems.  System A for example would be some preload step in my case some initial stresses.  Connect to system B allows me to bring stress, strains, or mesh deformation.  Caveat I'm looking at an older analysis and haven’t done this in a bit.  I might be missing a step or a critical point in here.  It gives you a start.

I looked at the APDL in the ds.dat file as well.  Here is some of it below. This is for importing stress on elements.

inistate,set,csys,0
inistate,set,dtyp,s
inistate,define,1,,,, Cxx, Cyy, Czz, Cxy, Cyz, Cxz (Stress (S), strain (EPEL), or plastic strain (EPPL) values)

Hope that gives some help.

Regards
Will

William Seppelt, PE
CAE Engineer
Validation and Release
BorgWarner Emissions, Thermal and Turbo Systems
Desk: +1 (828) 650-7479

wseppelt@borgwarner.com

-----Original Message-----
From: Bohlen, Dan (GE Aerospace, US) via Xansys xansys-temp@list.xansys.org
Sent: Tuesday, April 15, 2025 1:55 PM
To: XANSYS Mailing List Home xansys-temp@list.xansys.org
Cc: Bohlen, Dan (GE Aerospace, US) dan.bohlen@geaerospace.com
Subject: [Xansys] Re: playing with inistate Ansys 2024

⚠  EXTERNAL SENDER

Well, without saying TOO much.  I have a part at rest, but there are some residual strains baked into the part due to manufacturing.  Our supplier gives us a set of plastic strains we apply to the model and then we do our standard analysis.

I found some examples in the verification manual.  I think my biggest issue now is I'm not sure how to translate what we get from the supplier to the NISTATE command.  I tried a 1 element model and it would converge when I put the strains on the way I thought they should go.

Hoping to get a PhD engineering mechanics guy here to look at it.  I'm not even sure how you put plastic strains on a model - wouldn't it have to be elastic+plastic strains?  Our in house program may take that into account.

Dan

-----Original Message-----
From: Keith DiRienz via Xansys xansys-temp@list.xansys.org
Sent: Monday, April 14, 2025 1:40 PM
To: xansys-temp@list.xansys.org
Cc: Keith DiRienz fea-technologies@cox.net
Subject: [Xansys] Re: playing with inistate Ansys 2024

Would an old fashioned prestress restart work for this case ?

Keith DiRienz, P.E.
FEA Technologies
Office: 949.910.7049

On 4/14/2025 7:20 AM, Bohlen, Dan (GE Aerospace, US) via Xansys wrote:

--

Keith DiRienz, P.E.
FEA Technologies
Office: 949.910.7049

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 _______________________________________________
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

I know the following might not be the best you’re looking for, but can your
supplier provide you with deformations instead of plastic strains (depends
on what sort of measurement system they have). If you have the deformations
maybe you can apply them to the model using CBDOF command.

I have seen some groups import the DIC-measured deformations of electronic
packages subjected to drop test into their models using submodeling
technique (i.e., CBDOF) to solve for strains and stresses.

Good luck!
Mohammad

---====
Mohammad A Gharaibeh, Ph.D.
Associate Professor
Department of Mechanical Engineering
The Hashemite University
P.O. Box 330127
Zarqa, 13133, Jordan
Tel: +962 - 5 - 390 3333 Ext. 4771
Fax: +962 - 5 - 382 6348

---====

On Tue, 15 Apr 2025 at 8:54 PM Bohlen, Dan (GE Aerospace, US) via Xansys <
xansys-temp@list.xansys.org> wrote:

Dan,

You can use INISTATE command to define your initial strains based on a cloud of data points which we call mesh-independent initial-state, ADPL handles the mapping of this data to the finite element model internally. INISTATE has evolved beyond its original purpose of defining initial stress. There is a whole chapter about the initial state in APDL advanced analysis guide with many examples of various applications. I am copying you an example here

! Create a mesh-independent data file
*create,data,ist
/dtyp,epel
/idat,1,coor,1,X
/idat,2,coor,2,Y

/ddat,1,epel,1,XX
/ddat,2,epel,2,YY
/ddat,3,epel,3,XY

0,0,1e-4,0,0
0,1,1e-4,0,0
1,0,3e-4,0,0
1,1,3e-4,0,0
*end

/prep7
et,1,183
keyo,1,1,1
keyopt,1,3,3          ! Plane stress with thickness
r,1,.1

keyo,1,6,0

tb,elas,1
tbdat,,1e6,0.5

ex_1= 14E6
et_1 = 1.2E6
ep_1 = ex_1et_1/(ex_1-et_1)
yp=14e61.2E6/(14e6-1.2E6)

rect,0,1,0,1

lesiz,all,1,,
amesh,1

elist

/solu
inis,read,data,ist,,mapi
/out
inis,list,all
inis,list,glob
!/out,scratch

nsel,s,loc,x,0
nsel,a,loc,x,1
d,all,ux

nsel,s,loc,x,0
nsel,r,loc,y,0
d,all,uy
allsel,all
solve

/post1
set,last
/out
presol,epel
presol,s

Regards,
Guoyu

From: Bohlen, Dan (GE Aerospace, US) via Xansys xansys-temp@list.xansys.org
Sent: Tuesday, April 15, 2025 1:54 PM
To: XANSYS Mailing List Home xansys-temp@list.xansys.org
Cc: Bohlen, Dan (GE Aerospace, US) dan.bohlen@geaerospace.com
Subject: [Xansys] Re: playing with inistate Ansys 2024

[External Sender]

Well, without saying TOO much.  I have a part at rest, but there are some residual strains baked into the part due to manufacturing.  Our supplier gives us a set of plastic strains we apply to the model and then we do our standard analysis.

I found some examples in the verification manual.  I think my biggest issue now is I'm not sure how to translate what we get from the supplier to the NISTATE command.  I tried a 1 element model and it would converge when I put the strains on the way I thought they should go.

Hoping to get a PhD engineering mechanics guy here to look at it.  I'm not even sure how you put plastic strains on a model - wouldn't it have to be elastic+plastic strains?  Our in house program may take that into account.

Dan

-----Original Message-----
From: Keith DiRienz via Xansys xansys-temp@list.xansys.org
Sent: Monday, April 14, 2025 1:40 PM
To: xansys-temp@list.xansys.org
Cc: Keith DiRienz fea-technologies@cox.net
Subject: [Xansys] Re: playing with inistate Ansys 2024

Would an old fashioned prestress restart work for this case ?

Keith DiRienz, P.E.
FEA Technologies
Office: 949.910.7049

On 4/14/2025 7:20 AM, Bohlen, Dan (GE Aerospace, US) via Xansys wrote:

--

Keith DiRienz, P.E.
FEA Technologies
Office: 949.910.7049

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

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