Thanks for the replies on this one.

With some help from tech support, I was able to get this to work.  For those interested…

Under “Analysis Settings” I needed “Number of Steps” to be “1”
Under “Commands (APDL)” I needed “Issue Solve Command” to be “No”

Thanks,

Jim

[cid:image001.png@01D9BFBD.10CD6280]
James J. Patterson, PhD.
Principal Vehicle Systems Engineer
Trailer Commercial Vehicle Systems
2070 Industrial Place S.E.  Canton, OH 44707
ph. 330 489 0095  |  fax 330 489 1961
jpatterson@hendrickson-intl.commailto:jpatterson@hendrickson-intl.com
www.hendrickson-intl.com
[cid:image002.gif@01D9BFBD.10CD6280]

From: Caba, Aaron C (US) via Xansys xansys-temp@list.xansys.org
Sent: Wednesday, July 26, 2023 12:19 PM
To: XANSYS Mailing List Home xansys-temp@list.xansys.org
Cc: Caba, Aaron C (US) aaron.caba@baesystems.com
Subject: [Xansys] Re: Using LSSOLVE in WB...

James, My guess is after you manually run the solve with 'lssolve', the ds. dat file generated by Mechanical has another 'solve' command tacked on after your command snip. This is where you are getting 2 extra LS6 & LS7. If this is the case,
ZjQcmQRYFpfptBannerStart
[H] IT Security: This Message Is From an External Sender
Warning: This message came from someone outside of Hendrickson
Report Suspicious  https://us-phishalarm-ewt.proofpoint.com/EWT/v1/HXcklc0VomgEZw!3G9yYh7OjSXssYluWnGm3MMIwzJt-hvgjXUfWBAHT7-TMVn8uY_4ipmnLrwmIspfE953Q2gbYocx4EEiU7U1RhJ8b2mxLqEqvhdDLfDrixU2JOxnRWedQffGbXJE$  ‌
ZjQcmQRYFpfptBannerEnd

James,

My guess is after you manually run the solve with 'lssolve', the ds.dat file generated by Mechanical has another 'solve' command tacked on after your command snip.  This is where you are getting 2 extra LS6 & LS7.  If this is the case, you can just end your snip with the 'fini' command to prevent the 'solve' command from functioning.  Other times I've used *abbr,solve,allsel to disable solve.

To find the ds.dat file:  right-click on the 'Solution' branch and 'Open Solver Files Directory'

When I've hijacked Mechanical's solve process with command snips I found it necessary to ensure the # of steps and step times defined in Mechanical exactly matched those produced by my command snips.  If not, Mechanical can get really confused when displaying results.  If you aren't viewing the results in Mechanical you can ignore this requirement.

Aaron C. Caba, Ph.D.

Sr. Principal R&D Engineer

BAE Systems, Inc.

4050 Peppers Ferry Road, Radford VA 24143-0100

https://urldefense.com/v3/http://www.baesystems.com;!!HXcklc0VomgEZw!4s_T5fLHO7O35mojgZ-FnAcIvbdM5eaPBrnachuqiS_eM9-PLRFYyEWiH1EYUv4pBEXiF87BF_XuchaGM5GX5wetPjFZ-_6BF8A$https://urldefense.com/v3/__http:/www.baesystems.com__;!!HXcklc0VomgEZw!4s_T5fLHO7O35mojgZ-FnAcIvbdM5eaPBrnachuqiS_eM9-PLRFYyEWiH1EYUv4pBEXiF87BF_XuchaGM5GX5wetPjFZ-_6BF8A$

-----Original Message-----

From: Patterson, James <jpatterson@hendrickson-intl.commailto:jpatterson@hendrickson-intl.com>

Sent: Tuesday, July 25, 2023 9:42 AM

To: XANSYS Mailing List Home <xansys-temp@list.xansys.orgmailto:xansys-temp@list.xansys.org>

Subject: [Xansys] Using LSSOLVE in WB...

External Email Alert

This email has been sent from an account outside of the BAE Systems network.

Please treat the email with caution, especially if you are requested to click on a link, decrypt/open an attachment, or enable macros.  For further information on how to spot phishing, access “Cybersecurity OneSpace Page” and report phishing by clicking the button “Report Phishing” on the Outlook toolbar.

Good Morning,

I’m an ANSYS Classic guy but have a project that wants to be in WB, so I’m trying to get it to work as I want.  Prepare for a long (but interesting!) story…

1. I have a large structure where I’m interested in stresses/life at a small detail.

 *   Eventually I’ll get to a submodel.

2. The loading I’ll apply to this structure will come from an ADAMS multibody dynamics simulation.

 *   A full vehicle in various road events.

3. The workflow I’m trying is…

 *   Create a course model of the structure in WB.

 *   Use WB to create a flex body (modal neutral file) for use in ADAMS.



                                                i.     This is done in a “Modal” system in WB.



                                               ii.     Includes meshing and creation of required Remote Points.



 *   Import and apply this flex body in my ADAMS model.

 *   Make my run and export the loads on the flex body at several times of interest.



                                                i.     This is a really nice feature in ADAMS, as it makes a text file of ANSYS commands.



                                               ii.     It includes “LSWRITE” commands at each time point/loadstep.



                                              iii.     For this test, there are two loadsteps, t=1 and t=5, but it could be more in the future.



                                              iv.     See example file below.



 *   Have the modal system above feed a new structural system on the project page.

 *   Use a command object in the structural system to read the load file generated by ADAMS.



                                                i.     /input,FELoads,mac,C:\ADAMS_2023\MyTest



                                               ii.     time,1



                                              iii.     lssolve,1,2

This is where the trouble starts.

1. In the “Analysis Settings” details I specify “Number of steps” as 2.

 *   I have loads for t=1 and t=5.

2. When I hit solve, I get results at LS1 and LS5 as expected, but it then creates a repeat of LS5 twice for an LS6 and LS7 (???).

I’ve been trying different combinations of…

1. Using LSSOLVE or not

2. Setting TIME or not

3. Setting Number of Steps or not.

Have not stumbled onto the right combination.  Thoughts…???

Thanks,

Jim

Example loads exported from ADAMS…

!

!                    ********      A N S Y S      ********

!                    ****** LOADS DATA SET FRAGMENT ******

!                    Load File Created From Adams Analysis

!                    TO BE MERGED WITH  ANSYS INPUT FILE!

!                    Created:  Mon Jul 24 15:36:40 2023

!                    Number of Load Cases: 2

!                    Units: Mass  = pound_mass

!                            Length = inch

!                            Force  = pound_force

!                            Time  = sec

!                    *************************************

!

! Load Point Information  (Global Reference Frame):

! Node ID  Adams ID      X            Y            Z        Marker Label

! -------- -------- ------------ ------------ ------------ ------------

!        1        1  1.50000e+00  0.00000e+00  0.00000e+00 MARKER_1

!        2        3  1.65000e+01  2.50000e-01  0.00000e+00 MARKER_3

!

! Load Point Information  (FEA Reference Frame):

! Node ID  Adams ID      X            Y            Z        Marker Label

! -------- -------- ------------ ------------ ------------ ------------

!        1        1  1.50000e+00  0.00000e+00  0.00000e+00 MARKER_1

!        2        3  1.65000e+01  2.50000e-01  0.00000e+00 MARKER_3

!

!

! LOAD CASE = 1

!

TIME, 1.00000e+00

FDEL, ALL

ACEL,-3.07068e-01, 3.86088e+02, 0.00000e+00 OMEGA, 0.00000e+00, 0.00000e+00, 0.00000e+00 DOMEGA, 0.00000e+00, 0.00000e+00, 0.00000e+00 F, 1, FX,-4.46899e-03 F, 1, FY, 5.61904e+00 F, 1, MZ, 4.21435e+01 LSWRITE !

! LOAD CASE = 2

!

TIME, 5.00000e+00

FDEL, ALL

ACEL, 1.37511e+01, 3.85845e+02, 1.06758e-04 OMEGA, 0.00000e+00, 0.00000e+00, 0.00000e+00 DOMEGA, 0.00000e+00, 0.00000e+00,-3.45181e-04 F, 1, FX,-3.36153e+00 F, 1, FY,-9.43211e+01 F, 1, MY, 4.03109e-04 F, 1, MZ,-1.45596e+03 F, 2, FX, 3.56166e+00 F, 2, FY, 9.99366e+01 LSWRITE

[cid:image001.png@01D9BED8.E6B671B0]

James J. Patterson, PhD.

Principal Vehicle Systems Engineer

Trailer Commercial Vehicle Systems

2070 Industrial Place S.E.  Canton, OH 44707

ph. 330 489 0095  |  fax 330 489 1961

jpatterson@hendrickson-intl.com<mailto:jpatterson@hendrickson-intl.commailto:jpatterson@hendrickson-intl.com%3cmailto:jpatterson@hendrickson-intl.com>

http://www.hendrickson-intl.com

                                                     [cid:image002.gif@01D9BED8.E6B671B0]

The contents of this message may be privileged and confidential. Therefore, if this message has been received in error, please delete it without reading it. Your receipt of this message is not intended to waive any applicable privilege. Please do not disseminate this message without the permission of the author.

Xansys mailing list -- xansys-temp@list.xansys.orgmailto:xansys-temp@list.xansys.org

To unsubscribe send an email to xansys-temp-leave@list.xansys.orgmailto: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.ukmailto:xansys-mod@tynecomp.co.uk and not to the list

James,

When in WB, if several number of steps are defined in Analysis Settings, when you use a command object you can chose the Step Selection Mode (=> at what step you want those commands to be affected: First, All, Last or by step Number).

I think in your case you could try to specify First and insert /EOF at the end of your command object so to avoid any further actions beyond that.
Prior to hit WB solve button, you may ask to write down the input file (ds.dat) (Solution Tab> Write Input File) so you can have a look at what exactly will be sent to the solver.

How do you do in ADAMS to export the loads on the flex body?

Regards,

Carles SAGUÉS MITJANA

BOBST
BU Sheet Fed R&D Support
Numerical Simulation Expert & Material Adviser
Email: carles.saguesmitjana@bobst.com

-----Original Message-----
From: Patterson, James jpatterson@hendrickson-intl.com
Sent: Tuesday, July 25, 2023 3:42 PM
To: XANSYS Mailing List Home xansys-temp@list.xansys.org
Subject: [Xansys] Using LSSOLVE in WB...

Good Morning,

I'm an ANSYS Classic guy but have a project that wants to be in WB, so I'm trying to get it to work as I want.  Prepare for a long (but interesting!) story...

1. I have a large structure where I'm interested in stresses/life at a small detail.
   *  Eventually I'll get to a submodel.

2. The loading I'll apply to this structure will come from an ADAMS multibody dynamics simulation.
   *  A full vehicle in various road events.

3. The workflow I'm trying is...
   *  Create a course model of the structure in WB.
   *  Use WB to create a flex body (modal neutral file) for use in ADAMS.

                                             i.     This is done in a "Modal" system in WB.
   
                                            ii.     Includes meshing and creation of required Remote Points.
   

 *   Import and apply this flex body in my ADAMS model.
 *   Make my run and export the loads on the flex body at several times of interest.

                                                i.     This is a really nice feature in ADAMS, as it makes a text file of ANSYS commands.

                                               ii.     It includes "LSWRITE" commands at each time point/loadstep.

                                              iii.     For this test, there are two loadsteps, t=1 and t=5, but it could be more in the future.

                                              iv.     See example file below.

 *   Have the modal system above feed a new structural system on the project page.
 *   Use a command object in the structural system to read the load file generated by ADAMS.

                                                i.     /input,FELoads,mac,C:\ADAMS_2023\MyTest

                                               ii.     time,1

                                              iii.     lssolve,1,2

This is where the trouble starts.

1. In the "Analysis Settings" details I specify "Number of steps" as 2.
   *  I have loads for t=1 and t=5.
2. When I hit solve, I get results at LS1 and LS5 as expected, but it then creates a repeat of LS5 twice for an LS6 and LS7 (???).

I've been trying different combinations of...

1. Using LSSOLVE or not
2. Setting TIME or not
3. Setting Number of Steps or not.

Have not stumbled onto the right combination.  Thoughts...???

Thanks,

Jim

Example loads exported from ADAMS...

!
!                    ********      A N S Y S      ********
!                    ****** LOADS DATA SET FRAGMENT ******
!                    Load File Created From Adams Analysis
!                    TO BE MERGED WITH  ANSYS INPUT FILE!
!                    Created:  Mon Jul 24 15:36:40 2023
!                    Number of Load Cases: 2
!                    Units: Mass  = pound_mass
!                            Length = inch
!                            Force  = pound_force
!                            Time  = sec
!                    *************************************
!
! Load Point Information  (Global Reference Frame):
! Node ID  Adams ID      X            Y            Z        Marker Label
! -------- -------- ------------ ------------ ------------ ------------
!        1        1  1.50000e+00  0.00000e+00  0.00000e+00 MARKER_1
!        2        3  1.65000e+01  2.50000e-01  0.00000e+00 MARKER_3
!
! Load Point Information  (FEA Reference Frame):
! Node ID  Adams ID      X            Y            Z        Marker Label
! -------- -------- ------------ ------------ ------------ ------------
!        1        1  1.50000e+00  0.00000e+00  0.00000e+00 MARKER_1
!        2        3  1.65000e+01  2.50000e-01  0.00000e+00 MARKER_3
!
!
! LOAD CASE = 1
!
TIME, 1.00000e+00
FDEL, ALL
ACEL,-3.07068e-01, 3.86088e+02, 0.00000e+00 OMEGA, 0.00000e+00, 0.00000e+00, 0.00000e+00 DOMEGA, 0.00000e+00, 0.00000e+00, 0.00000e+00 F, 1, FX,-4.46899e-03 F, 1, FY, 5.61904e+00 F, 1, MZ, 4.21435e+01 LSWRITE !
! LOAD CASE = 2
!
TIME, 5.00000e+00
FDEL, ALL
ACEL, 1.37511e+01, 3.85845e+02, 1.06758e-04 OMEGA, 0.00000e+00, 0.00000e+00, 0.00000e+00 DOMEGA, 0.00000e+00, 0.00000e+00,-3.45181e-04 F, 1, FX,-3.36153e+00 F, 1, FY,-9.43211e+01 F, 1, MY, 4.03109e-04 F, 1, MZ,-1.45596e+03 F, 2, FX, 3.56166e+00 F, 2, FY, 9.99366e+01 LSWRITE

[cid:image001.png@01D9BED8.E6B671B0]
James J. Patterson, PhD.
Principal Vehicle Systems Engineer
Trailer Commercial Vehicle Systems
2070 Industrial Place S.E.  Canton, OH 44707
ph. 330 489 0095  |  fax 330 489 1961
jpatterson@hendrickson-intl.commailto:jpatterson@hendrickson-intl.com
http://www.hendrickson-intl.com/
[cid:image002.gif@01D9BED8.E6B671B0]

The contents of this message may be privileged and confidential. Therefore, if this message has been received in error, please delete it without reading it. Your receipt of this message is not intended to waive any applicable privilege. Please do not disseminate this message without the permission of the author.

Dear Mr. Patterson,
I have replicated your use case.
I have used the following Commands (APDL) object in Workbench

/input,FELoads,mac,C:\ADAMS_2023\MyTest
lssolve,1,2
/eof

I have specified 1 as Number of Step in the Analysis Settings
I have got a result file which contains 2 load steps and that can be processed in Workbench's postprocessor. The results seem reasonable.

Best regards
Riccardo Testi

Development and Strategies
2 Wheeler Engines Technical Centre
Piaggio & C. S.p.A
Viale Rinaldo Piaggio, 25
56025 Pontedera (Pisa) - ITALY
Phone:  +39 0587 272850
Fax:        +39 0587 272010
Mobile: +39 339 7241918
E-mail:    riccardo.testi@piaggio.com

-----Original Message-----
From: Patterson, James jpatterson@hendrickson-intl.com
Sent: martedì 25 luglio 2023 15:42
To: XANSYS Mailing List Home xansys-temp@list.xansys.org
Subject: [Xansys] Using LSSOLVE in WB...

CAUTION:This email originated from outside the Piaggio Group. Do not click links or open attachments unless you recognize the sender and know the content is safe.

Good Morning,

I’m an ANSYS Classic guy but have a project that wants to be in WB, so I’m trying to get it to work as I want.  Prepare for a long (but interesting!) story…

1. I have a large structure where I’m interested in stresses/life at a small detail.
   *  Eventually I’ll get to a submodel.

2. The loading I’ll apply to this structure will come from an ADAMS multibody dynamics simulation.
   *  A full vehicle in various road events.

3. The workflow I’m trying is…
   *  Create a course model of the structure in WB.
   *  Use WB to create a flex body (modal neutral file) for use in ADAMS.

                                             i.     This is done in a “Modal” system in WB.
   
                                            ii.     Includes meshing and creation of required Remote Points.
   

 *   Import and apply this flex body in my ADAMS model.
 *   Make my run and export the loads on the flex body at several times of interest.

                                                i.     This is a really nice feature in ADAMS, as it makes a text file of ANSYS commands.

                                               ii.     It includes “LSWRITE” commands at each time point/loadstep.

                                              iii.     For this test, there are two loadsteps, t=1 and t=5, but it could be more in the future.

                                              iv.     See example file below.

 *   Have the modal system above feed a new structural system on the project page.
 *   Use a command object in the structural system to read the load file generated by ADAMS.

                                                i.     /input,FELoads,mac,C:\ADAMS_2023\MyTest

                                               ii.     time,1

                                              iii.     lssolve,1,2

This is where the trouble starts.

1. In the “Analysis Settings” details I specify “Number of steps” as 2.
   *  I have loads for t=1 and t=5.
2. When I hit solve, I get results at LS1 and LS5 as expected, but it then creates a repeat of LS5 twice for an LS6 and LS7 (???).

I’ve been trying different combinations of…

1. Using LSSOLVE or not
2. Setting TIME or not
3. Setting Number of Steps or not.

Have not stumbled onto the right combination.  Thoughts…???

Thanks,

Jim

Example loads exported from ADAMS…

!
!                    ********      A N S Y S      ********
!                    ****** LOADS DATA SET FRAGMENT ******
!                    Load File Created From Adams Analysis
!                    TO BE MERGED WITH  ANSYS INPUT FILE!
!                    Created:  Mon Jul 24 15:36:40 2023
!                    Number of Load Cases: 2
!                    Units: Mass  = pound_mass
!                            Length = inch
!                            Force  = pound_force
!                            Time  = sec
!                    *************************************
!
! Load Point Information  (Global Reference Frame):
! Node ID  Adams ID      X            Y            Z        Marker Label
! -------- -------- ------------ ------------ ------------ ------------
!        1        1  1.50000e+00  0.00000e+00  0.00000e+00 MARKER_1
!        2        3  1.65000e+01  2.50000e-01  0.00000e+00 MARKER_3
!
! Load Point Information  (FEA Reference Frame):
! Node ID  Adams ID      X            Y            Z        Marker Label
! -------- -------- ------------ ------------ ------------ ------------
!        1        1  1.50000e+00  0.00000e+00  0.00000e+00 MARKER_1
!        2        3  1.65000e+01  2.50000e-01  0.00000e+00 MARKER_3
!
!
! LOAD CASE = 1
!
TIME, 1.00000e+00
FDEL, ALL
ACEL,-3.07068e-01, 3.86088e+02, 0.00000e+00 OMEGA, 0.00000e+00, 0.00000e+00, 0.00000e+00 DOMEGA, 0.00000e+00, 0.00000e+00, 0.00000e+00 F, 1, FX,-4.46899e-03 F, 1, FY, 5.61904e+00 F, 1, MZ, 4.21435e+01 LSWRITE !
! LOAD CASE = 2
!
TIME, 5.00000e+00
FDEL, ALL
ACEL, 1.37511e+01, 3.85845e+02, 1.06758e-04 OMEGA, 0.00000e+00, 0.00000e+00, 0.00000e+00 DOMEGA, 0.00000e+00, 0.00000e+00,-3.45181e-04 F, 1, FX,-3.36153e+00 F, 1, FY,-9.43211e+01 F, 1, MY, 4.03109e-04 F, 1, MZ,-1.45596e+03 F, 2, FX, 3.56166e+00 F, 2, FY, 9.99366e+01 LSWRITE

[cid:image001.png@01D9BED8.E6B671B0]
James J. Patterson, PhD.
Principal Vehicle Systems Engineer
Trailer Commercial Vehicle Systems
2070 Industrial Place S.E.  Canton, OH 44707
ph. 330 489 0095  |  fax 330 489 1961
jpatterson@hendrickson-intl.commailto:jpatterson@hendrickson-intl.com
https://urlsand.esvalabs.com/?u=http%3A%2F%2Fwww.hendrickson-intl.com&e=6e97a7e3&h=fdf0b464&f=y&p=y
[cid:image002.gif@01D9BED8.E6B671B0]

The contents of this message may be privileged and confidential. Therefore, if this message has been received in error, please delete it without reading it. Your receipt of this message is not intended to waive any applicable privilege. Please do not disseminate this message without the permission of the author.