Hello Ansys experts, I have a 3D model_1 (consider an 'L' shaped 3D plate) for which the nodal pressures on the outer surfaces are retrieved and saved in a text file (figure on the left) and this model is meshed with triangular elements. Another 3D model_2 (segments of model_1 attached together to form a part) is modelled where the nodal pressures from model_1 are to be applied along with other boundary conditions to calculate the stresses (figure on the right). Please note that the segment dimensions of both models are maintained the same as shown in the attached document for the sample figure of the models. Kindly suggest how to proceed with applying the nodal pressures of one model to the other in order to calculate the stresses in Ansys apdl. Findings: through some of the articles and the discussions on different forums, I understood that SFA command will help in this scenario, please suggest a suitable approach from your expertise. Also, let me know in case of any other information is required. Thanks & Regards, Shravani Bojja FUAS

You might want to look up the submodeling technique. You will be able to transfer BCs from model 1 to model 2. Dig up the submodeling in ANSYS advanced analysis guide. Good luck! On Thursday, November 3, 2022, shbo4183 <shravani.bojja@stud.hs-flensburg.de> wrote: > Hello Ansys experts, > > I have a 3D model_1 (consider an 'L' shaped 3D plate) for which the nodal > pressures on the outer surfaces are retrieved and saved in a text file > (figure on the left) and this model is meshed with triangular elements. > Another 3D model_2 (segments of model_1 attached together to form a part) > is modelled where the nodal pressures from model_1 are to be applied along > with other boundary conditions to calculate the stresses (figure on the > right). > > Please note that the segment dimensions of both models are maintained the > same as shown in the attached document for the sample figure of the models. > > Kindly suggest how to proceed with applying the nodal pressures of one > model to the other in order to calculate the stresses in Ansys apdl. > > Findings: through some of the articles and the discussions on different > forums, I understood that SFA command will help in this scenario, please > suggest a suitable approach from your expertise. Also, let me know in case > of any other information is required. > > > Thanks & Regards, > Shravani Bojja > FUAS -- ===================================== 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 =====================================

If you are using APDL (the cutting edge of 1970's technology) and have dissimilar meshes, look at the *moper,,map for mapping as shown in https://ansys-net.svsfem.cz/macros/mapme.mac If you are using Workbench this task is trivially easy using an External Data system. It will read the text file, perform mapping between dissimilar meshes, apply coordinate transformations, and take care of any unit conversions - all automagically. No lines of code needed. Aaron C. Caba, Ph.D. Sr. Principal R&D Engineer II BAE Systems, Inc. | Ordnance Systems, Inc. Office: +1 540 639 7086 | Mobile: +1 540 230 3906 | E-mail: aaron.caba@baesystems.com | Mail: 4050 Peppers Ferry Road, Radford VA 24143-0100 www.baesystems.com -----Original Message----- From: shbo4183 <shravani.bojja@stud.hs-flensburg.de> Sent: Thursday, November 3, 2022 6:36 AM To: Xansys Temp <xansys-temp@list.xansys.org> Subject: [Xansys] Applying Bc's in Ansys APDL Hello Ansys experts, I have a 3D model_1 (consider an 'L' shaped 3D plate) for which the nodal pressures on the outer surfaces are retrieved and saved in a text file (figure on the left) and this model is meshed with triangular elements. Another 3D model_2 (segments of model_1 attached together to form a part) is modelled where the nodal pressures from model_1 are to be applied along with other boundary conditions to calculate the stresses (figure on the right). Please note that the segment dimensions of both models are maintained the same as shown in the attached document for the sample figure of the models. Kindly suggest how to proceed with applying the nodal pressures of one model to the other in order to calculate the stresses in Ansys apdl. Findings: through some of the articles and the discussions on different forums, I understood that SFA command will help in this scenario, please suggest a suitable approach from your expertise. Also, let me know in case of any other information is required. Thanks & Regards, Shravani Bojja FUAS

On 03.11.2022 13:43, Caba, Aaron (US) via Xansys wrote: > If you are using APDL (the cutting edge of 1970's technology) and have > dissimilar meshes, look at the *moper,,map for mapping as shown in > https://ansys-net.svsfem.cz/macros/mapme.mac > > > If you are using Workbench this task is trivially easy using an > External Data system. It will read the text file, perform mapping > between dissimilar meshes, apply coordinate transformations, and take > care of any unit conversions - all automagically. No lines of code > needed. > > > > Aaron C. Caba, Ph.D. > > Sr. Principal R&D Engineer II > > BAE Systems, Inc. | Ordnance Systems, Inc. > > > > Office: +1 540 639 7086 | Mobile: +1 540 230 3906 | E-mail: > aaron.caba@baesystems.com | Mail: 4050 Peppers Ferry Road, Radford VA > 24143-0100 > > www.baesystems.com > > > > > > -----Original Message----- > From: shbo4183 <shravani.bojja@stud.hs-flensburg.de> > Sent: Thursday, November 3, 2022 6:36 AM > To: Xansys Temp <xansys-temp@list.xansys.org> > Subject: [Xansys] Applying Bc's in Ansys APDL > > > > Hello Ansys experts, > > > > I have a 3D model_1 (consider an 'L' shaped 3D plate) for which the > nodal pressures on the outer surfaces are retrieved and saved in a > text file (figure on the left) and this model is meshed with > triangular elements. Another 3D model_2 (segments of model_1 attached > together to form a part) is modelled where the nodal pressures from > model_1 are to be applied along with other boundary conditions to > calculate the stresses (figure on the right). > > > > Please note that the segment dimensions of both models are maintained > the same as shown in the attached document for the sample figure of > the models. > > > > Kindly suggest how to proceed with applying the nodal pressures of one > model to the other in order to calculate the stresses in Ansys apdl. > > > > Findings: through some of the articles and the discussions on > different forums, I understood that SFA command will help in this > scenario, please suggest a suitable approach from your expertise. > Also, let me know in case of any other information is required. > > > > > > Thanks & Regards, > > Shravani Bojja > > FUAS > _______________________________________________ > 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 Hello All, I would like to know more about SFA command usage with the help of table boundary conditions. The aim of the task is to apply the pressures at each node of an area which forms a boundary condition for further solving the model. With the below values read into a table (total_pres) for example, the sfa command is written as sfa,tot_area,,pres,%total_pres% Node number Pressure 1 25 2 20 3 15 4 12.5 5 16 Questions: 1. How to introduce nodal pressures onto the selected area using the SFA command 2. what all values are to be included in the table data? Are the node number and the pressure values will suffice, or the coordinate values are to be considered? 3. How is the pressure applied to the selected areas? is the total pressure of all these nodes summed up and then applied or? Kindly suggest to me how to proceed further, as the help document has a limited description of the same. Thanks & Regards, Shravani Bojja FUAS

SFA command is more related to apply a constant PRessure to existing Geometric Surfaces the command that suits to your needs is the SF command (for Nodes): *SF*, *Nlist*, *Lab*, *VALUE*, *VALUE2*, – ,*MESHFLAG* *Defines surface loads on nodes.* In order to define a variable pressure over nodes: 1) Create an array with the size equal to the maximum node number in the model *get, nmax, node,,num, max *dim, pressnodes, array, nmax 2) fill the pressures according to the position of the array equal to the node number (the rest of array positions will be zero) pressnodes(NOdenumer)=PressValue 3) apply the pressure array over your mesh: sffun, PRES, pressnodes(1) Iker Gomez Vazquez Structural Analysis @ ITP Aero Mexico El lun, 14 nov 2022 a las 3:02, shbo4183 (< shravani.bojja@stud.hs-flensburg.de>) escribió: > On 03.11.2022 13:43, Caba, Aaron (US) via Xansys wrote: > > If you are using APDL (the cutting edge of 1970's technology) and have > > dissimilar meshes, look at the *moper,,map for mapping as shown in > > https://ansys-net.svsfem.cz/macros/mapme.mac > > > > > > If you are using Workbench this task is trivially easy using an > > External Data system. It will read the text file, perform mapping > > between dissimilar meshes, apply coordinate transformations, and take > > care of any unit conversions - all automagically. No lines of code > > needed. > > > > > > > > Aaron C. Caba, Ph.D. > > > > Sr. Principal R&D Engineer II > > > > BAE Systems, Inc. | Ordnance Systems, Inc. > > > > > > > > Office: +1 540 639 7086 | Mobile: +1 540 230 3906 | E-mail: > > aaron.caba@baesystems.com | Mail: 4050 Peppers Ferry Road, Radford VA > > 24143-0100 > > > > www.baesystems.com > > > > > > > > > > > > -----Original Message----- > > From: shbo4183 <shravani.bojja@stud.hs-flensburg.de> > > Sent: Thursday, November 3, 2022 6:36 AM > > To: Xansys Temp <xansys-temp@list.xansys.org> > > Subject: [Xansys] Applying Bc's in Ansys APDL > > > > > > > > Hello Ansys experts, > > > > > > > > I have a 3D model_1 (consider an 'L' shaped 3D plate) for which the > > nodal pressures on the outer surfaces are retrieved and saved in a > > text file (figure on the left) and this model is meshed with > > triangular elements. Another 3D model_2 (segments of model_1 attached > > together to form a part) is modelled where the nodal pressures from > > model_1 are to be applied along with other boundary conditions to > > calculate the stresses (figure on the right). > > > > > > > > Please note that the segment dimensions of both models are maintained > > the same as shown in the attached document for the sample figure of > > the models. > > > > > > > > Kindly suggest how to proceed with applying the nodal pressures of one > > model to the other in order to calculate the stresses in Ansys apdl. > > > > > > > > Findings: through some of the articles and the discussions on > > different forums, I understood that SFA command will help in this > > scenario, please suggest a suitable approach from your expertise. > > Also, let me know in case of any other information is required. > > > > > > > > > > > > Thanks & Regards, > > > > Shravani Bojja > > > > FUAS > > _______________________________________________ > > 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 > > Hello All, > > I would like to know more about SFA command usage with the help of table > boundary conditions. > The aim of the task is to apply the pressures at each node of an area > which forms a boundary condition for further solving the model. > > With the below values read into a table (total_pres) for example, the > sfa command is written as sfa,tot_area,,pres,%total_pres% > > Node number Pressure > 1 25 > 2 20 > 3 15 > 4 12.5 > 5 16 > > Questions: > 1. How to introduce nodal pressures onto the selected area using the SFA > command > 2. what all values are to be included in the table data? Are the node > number and the pressure values will suffice, or the coordinate values > are to be considered? > 3. How is the pressure applied to the selected areas? is the total > pressure of all these nodes summed up and then applied or? > > Kindly suggest to me how to proceed further, as the help document has a > limited description of the same. > > Thanks & Regards, > Shravani Bojja > FUAS > _______________________________________________ > 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 > -- Iker Gómez Vázquez Santa Rita 102, #52 Queretaro 76230 Mexico Tfno. +52 442 2841569