Empathy List Archives

BD

Bohlen, Dan (GE, US)

Thu, Jan 18, 2024 2:03 PM

Hi All,

Running a an 3D E-P FBO analysis on a military fan shaft.

I have a model that ran with a legacy engine set of loads. Run checked out and matches field experience. The same model was run with a new application set of loads that were 50-100% higher and not surprisingly the model crashed at about 60% load.

I morphed the shaft to a more robust shape and the model is stopping at 92% load. So I think we might be close to usable design and looking for any tweaks to nudge the solution along.

Steps I'm taking:

Rerunning and dumping out results at some substeps before the model diverges to see what's happening.
Trying the STABILIZE command
Tried ARCLEN - didn't help

Not sure if mesh size can be an issue (too fine or too coarse).

Any thoughts or suggestions welcomed.

Charge code=ENG.110264-Y17P

Dan Bohlen
Senior Engineer, Stress Analysis
STAR review chairman, military structures
GE Aerospace
1 Neumann Way
Evendale, OH 45215 USA

Building B90 Column L 3.75
M/D H358 Cell 513-917-3402

Building 200 Desk Phone 3-8816

GE FOCUS: Safety, Quality, Delivery, Cost

"In God we trust, all others bring data." W Edwards Deming

[IMG_0492]

Hi All, Running a an 3D E-P FBO analysis on a military fan shaft. I have a model that ran with a legacy engine set of loads. Run checked out and matches field experience. The same model was run with a new application set of loads that were 50-100% higher and not surprisingly the model crashed at about 60% load. I morphed the shaft to a more robust shape and the model is stopping at 92% load. So I think we might be close to usable design and looking for any tweaks to nudge the solution along. Steps I'm taking: * Rerunning and dumping out results at some substeps before the model diverges to see what's happening. * Trying the STABILIZE command * Tried ARCLEN - didn't help Not sure if mesh size can be an issue (too fine or too coarse). Any thoughts or suggestions welcomed. Charge code=ENG.110264-Y17P Dan Bohlen Senior Engineer, Stress Analysis STAR review chairman, military structures GE Aerospace 1 Neumann Way Evendale, OH 45215 USA Building B90 Column L 3.75 M/D H358 Cell 513-917-3402 Building 200 Desk Phone 3-8816 GE FOCUS: Safety, Quality, Delivery, Cost "In God we trust, all others bring data." W Edwards Deming [IMG_0492]

DG

Diego Gorriz Sainz

Thu, Jan 18, 2024 2:52 PM

Hi, try to increase the mesh size only a little, sometimes this is useful.

Best regards

-----Mensaje original-----
De: Bohlen, Dan (GE, US) dan.bohlen@ge.com
Enviado el: jueves, 18 de enero de 2024 15:04
Para: @EDISON WORKS MECHANICAL_ANALYSIS EWMA@ge.com
CC: Zhu, Changming (GE Aerospace, US) changming.zhu@ge.com; Perivolarakis, Peter (GE Aerospace, US) peter.perivolarakis@ge.com
Asunto: [Xansys] Crowdsourcing: elastic-plastic model potentially buckling

ADVERTENCIA: Correo Externo [WARNING: External email]

Hi All,

Running a an 3D E-P FBO analysis on a military fan shaft.

I have a model that ran with a legacy engine set of loads. Run checked out and matches field experience. The same model was run with a new application set of loads that were 50-100% higher and not surprisingly the model crashed at about 60% load.

I morphed the shaft to a more robust shape and the model is stopping at 92% load. So I think we might be close to usable design and looking for any tweaks to nudge the solution along.

Steps I'm taking:

Rerunning and dumping out results at some substeps before the model diverges to see what's happening.
Trying the STABILIZE command
Tried ARCLEN - didn't help

Not sure if mesh size can be an issue (too fine or too coarse).

Any thoughts or suggestions welcomed.

Charge code=ENG.110264-Y17P

Dan Bohlen
Senior Engineer, Stress Analysis
STAR review chairman, military structures GE Aerospace
1 Neumann Way
Evendale, OH 45215 USA

Building B90 Column L 3.75
M/D H358 Cell 513-917-3402

Building 200 Desk Phone 3-8816

GE FOCUS: Safety, Quality, Delivery, Cost

"In God we trust, all others bring data." W Edwards Deming

[IMG_0492]

Hi, try to increase the mesh size only a little, sometimes this is useful. Best regards -----Mensaje original----- De: Bohlen, Dan (GE, US) <dan.bohlen@ge.com> Enviado el: jueves, 18 de enero de 2024 15:04 Para: @EDISON WORKS MECHANICAL_ANALYSIS <EWMA@ge.com> CC: Zhu, Changming (GE Aerospace, US) <changming.zhu@ge.com>; Perivolarakis, Peter (GE Aerospace, US) <peter.perivolarakis@ge.com> Asunto: [Xansys] Crowdsourcing: elastic-plastic model potentially buckling ADVERTENCIA: Correo Externo [WARNING: External email] Hi All, Running a an 3D E-P FBO analysis on a military fan shaft. I have a model that ran with a legacy engine set of loads. Run checked out and matches field experience. The same model was run with a new application set of loads that were 50-100% higher and not surprisingly the model crashed at about 60% load. I morphed the shaft to a more robust shape and the model is stopping at 92% load. So I think we might be close to usable design and looking for any tweaks to nudge the solution along. Steps I'm taking: * Rerunning and dumping out results at some substeps before the model diverges to see what's happening. * Trying the STABILIZE command * Tried ARCLEN - didn't help Not sure if mesh size can be an issue (too fine or too coarse). Any thoughts or suggestions welcomed. Charge code=ENG.110264-Y17P Dan Bohlen Senior Engineer, Stress Analysis STAR review chairman, military structures GE Aerospace 1 Neumann Way Evendale, OH 45215 USA Building B90 Column L 3.75 M/D H358 Cell 513-917-3402 Building 200 Desk Phone 3-8816 GE FOCUS: Safety, Quality, Delivery, Cost "In God we trust, all others bring data." W Edwards Deming [IMG_0492]

RS

Rod Scholl

Thu, Jan 18, 2024 3:09 PM

Hi Dan!

Consider turning on newton Raphson residuals to see if it failing at a contact region or joints, etc. (or if there are any other things to tweak at that location... also see if the location of the NR is jumping around which is indicative of other types of problems.

If it's not failing from NR -- and is element distortion... you have to tweak the mesh (and substep size)... we often have to do this over and over... it's seemingly random. Small mesh tweaks... a little bigger... a little smaller... step size a little bigger... a little smaller. Don't focus just on restarts... or if you do, go back a few steps... sometimes the last substep can't be proceeded from, but if you go back a few and then start solving it can help.

Not sure what your plastic materials are -- but maybe also avoid a (near)perfectly plastic region... it's better to have an unrealistically high tangent modulus/slope at the end of your curve, even out past the materials maximum elongation, then for ansys to try and solve that high deformation zone. So if you're using BKIN/MKIN you can have a little wing tip that goes up after max-elongation strain. Then after solving you can then just check for regions past your max elongation and know that it shoulda failed (you just didn't capture the actual failure event -- just the load it happens at). When the guesses for equilibrium iterations keep dipping their toes into a numerically unstable results (tangent modulus near-zero) then it starts putting up element distortion errors.

Hope that helps... and take solace in this oldie but a goodie:
https://epsilonfea.com/issue-1-january-2013/

Rod Scholl
Principal
Phone: 952-405-9710
Email: Rod.Scholl@EpsilonFEA.com
www.EpsilonFEA.com

-----Original Message-----
From: Diego Gorriz Sainz via Xansys xansys-temp@list.xansys.org
Sent: Thursday, January 18, 2024 8:52 AM
To: XANSYS Mailing List Home xansys-temp@list.xansys.org; @EDISON WORKS MECHANICAL_ANALYSIS EWMA@ge.com
Cc: Zhu, Changming (GE Aerospace, US) changming.zhu@ge.com; Perivolarakis, Peter (GE Aerospace, US) peter.perivolarakis@ge.com; Diego Gorriz Sainz diego.gorriz@pwh.es
Subject: [Xansys] Re: Crowdsourcing: elastic-plastic model potentially buckling

Hi, try to increase the mesh size only a little, sometimes this is useful.

Best regards

-----Mensaje original-----
De: Bohlen, Dan (GE, US) dan.bohlen@ge.com Enviado el: jueves, 18 de enero de 2024 15:04
Para: @EDISON WORKS MECHANICAL_ANALYSIS EWMA@ge.com
CC: Zhu, Changming (GE Aerospace, US) changming.zhu@ge.com; Perivolarakis, Peter (GE Aerospace, US) peter.perivolarakis@ge.com
Asunto: [Xansys] Crowdsourcing: elastic-plastic model potentially buckling

ADVERTENCIA: Correo Externo [WARNING: External email]

Hi All,

Running a an 3D E-P FBO analysis on a military fan shaft.

I have a model that ran with a legacy engine set of loads. Run checked out and matches field experience. The same model was run with a new application set of loads that were 50-100% higher and not surprisingly the model crashed at about 60% load.

I morphed the shaft to a more robust shape and the model is stopping at 92% load. So I think we might be close to usable design and looking for any tweaks to nudge the solution along.

Steps I'm taking:

Rerunning and dumping out results at some substeps before the model diverges to see what's happening.
Trying the STABILIZE command
Tried ARCLEN - didn't help

Not sure if mesh size can be an issue (too fine or too coarse).

Any thoughts or suggestions welcomed.

Charge code=ENG.110264-Y17P

Dan Bohlen
Senior Engineer, Stress Analysis
STAR review chairman, military structures GE Aerospace
1 Neumann Way
Evendale, OH 45215 USA

Building B90 Column L 3.75
M/D H358 Cell 513-917-3402

Building 200 Desk Phone 3-8816

GE FOCUS: Safety, Quality, Delivery, Cost

"In God we trust, all others bring data." W Edwards Deming

[IMG_0492]

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 Dan! Consider turning on newton Raphson residuals to see if it failing at a contact region or joints, etc. (or if there are any other things to tweak at that location... also see if the location of the NR is jumping around which is indicative of other types of problems. If it's not failing from NR -- and is element distortion... you have to tweak the mesh (and substep size)... we often have to do this over and over... it's seemingly random. Small mesh tweaks... a little bigger... a little smaller... step size a little bigger... a little smaller. Don't focus just on restarts... or if you do, go back a few steps... sometimes the last substep can't be proceeded from, but if you go back a few and then start solving it can help. Not sure what your plastic materials are -- but maybe also avoid a (near)perfectly plastic region... it's better to have an unrealistically high tangent modulus/slope at the end of your curve, even out past the materials maximum elongation, then for ansys to try and solve that high deformation zone. So if you're using BKIN/MKIN you can have a little wing tip that goes up after max-elongation strain. Then after solving you can then just check for regions past your max elongation and know that it shoulda failed (you just didn't capture the actual failure event -- just the load it happens at). When the guesses for equilibrium iterations keep dipping their toes into a numerically unstable results (tangent modulus near-zero) then it starts putting up element distortion errors. Hope that helps... and take solace in this oldie but a goodie: https://epsilonfea.com/issue-1-january-2013/ ______________________________ Rod Scholl Principal Phone: 952-405-9710 Email: Rod.Scholl@EpsilonFEA.com www.EpsilonFEA.com -----Original Message----- From: Diego Gorriz Sainz via Xansys <xansys-temp@list.xansys.org> Sent: Thursday, January 18, 2024 8:52 AM To: XANSYS Mailing List Home <xansys-temp@list.xansys.org>; @EDISON WORKS MECHANICAL_ANALYSIS <EWMA@ge.com> Cc: Zhu, Changming (GE Aerospace, US) <changming.zhu@ge.com>; Perivolarakis, Peter (GE Aerospace, US) <peter.perivolarakis@ge.com>; Diego Gorriz Sainz <diego.gorriz@pwh.es> Subject: [Xansys] Re: Crowdsourcing: elastic-plastic model potentially buckling Hi, try to increase the mesh size only a little, sometimes this is useful. Best regards -----Mensaje original----- De: Bohlen, Dan (GE, US) <dan.bohlen@ge.com> Enviado el: jueves, 18 de enero de 2024 15:04 Para: @EDISON WORKS MECHANICAL_ANALYSIS <EWMA@ge.com> CC: Zhu, Changming (GE Aerospace, US) <changming.zhu@ge.com>; Perivolarakis, Peter (GE Aerospace, US) <peter.perivolarakis@ge.com> Asunto: [Xansys] Crowdsourcing: elastic-plastic model potentially buckling ADVERTENCIA: Correo Externo [WARNING: External email] Hi All, Running a an 3D E-P FBO analysis on a military fan shaft. I have a model that ran with a legacy engine set of loads. Run checked out and matches field experience. The same model was run with a new application set of loads that were 50-100% higher and not surprisingly the model crashed at about 60% load. I morphed the shaft to a more robust shape and the model is stopping at 92% load. So I think we might be close to usable design and looking for any tweaks to nudge the solution along. Steps I'm taking: * Rerunning and dumping out results at some substeps before the model diverges to see what's happening. * Trying the STABILIZE command * Tried ARCLEN - didn't help Not sure if mesh size can be an issue (too fine or too coarse). Any thoughts or suggestions welcomed. Charge code=ENG.110264-Y17P Dan Bohlen Senior Engineer, Stress Analysis STAR review chairman, military structures GE Aerospace 1 Neumann Way Evendale, OH 45215 USA Building B90 Column L 3.75 M/D H358 Cell 513-917-3402 Building 200 Desk Phone 3-8816 GE FOCUS: Safety, Quality, Delivery, Cost "In God we trust, all others bring data." W Edwards Deming [IMG_0492] _______________________________________________ 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

JW

Joe Woodward

Thu, Jan 18, 2024 3:52 PM

Dan,

If your job is crashing due to element deformation issues, you could try the mesh rezoning.

Thank you,

Joe

Joe Woodward
Chief Engineer
Simulation Support

PADT, Inc.
www.PADTINC.com
480.813.4884 x156
480.813.4807 fax
joe.woodward@padtinc.com

Simulation - Product Development - Rapid Prototyping

For Your ANSYS Training/Mentoring Needs:
https://www.padtinc.com/support/software/training
https://www.padtinc.com/support/software/Mentoring

CONFIDENTIALITY NOTICE: This e-mail message and any attachments are for the sole use of the intended recipient(s) and may contain confidential and/or privileged information. Unless you are the intended recipient, you are hereby notified that copying, forwarding, printing or otherwise disseminating the information contained in or attached to this e-mail is strictly prohibited. If you are not the intended recipient, please notify the sender by telephone, and immediately and permanently delete and destroy all copies and printouts of this e-mail message and/or attachments.

-----Original Message-----
From: Bohlen, Dan (GE, US) dan.bohlen@ge.com
Sent: Thursday, January 18, 2024 7:04 AM
To: @EDISON WORKS MECHANICAL_ANALYSIS EWMA@ge.com
Cc: Zhu, Changming (GE Aerospace, US) changming.zhu@ge.com; Perivolarakis, Peter (GE Aerospace, US) peter.perivolarakis@ge.com
Subject: [Xansys] Crowdsourcing: elastic-plastic model potentially buckling

Hi All,

Running a an 3D E-P FBO analysis on a military fan shaft.

I have a model that ran with a legacy engine set of loads. Run checked out and matches field experience. The same model was run with a new application set of loads that were 50-100% higher and not surprisingly the model crashed at about 60% load.

I morphed the shaft to a more robust shape and the model is stopping at 92% load. So I think we might be close to usable design and looking for any tweaks to nudge the solution along.

Steps I'm taking:

Rerunning and dumping out results at some substeps before the model diverges to see what's happening.
Trying the STABILIZE command
Tried ARCLEN - didn't help

Not sure if mesh size can be an issue (too fine or too coarse).

Any thoughts or suggestions welcomed.

Charge code=ENG.110264-Y17P

Dan Bohlen
Senior Engineer, Stress Analysis
STAR review chairman, military structures GE Aerospace
1 Neumann Way
Evendale, OH 45215 USA

Building B90 Column L 3.75
M/D H358 Cell 513-917-3402

Building 200 Desk Phone 3-8816

GE FOCUS: Safety, Quality, Delivery, Cost

"In God we trust, all others bring data." W Edwards Deming

[IMG_0492]

Dan, If your job is crashing due to element deformation issues, you could try the mesh rezoning. Thank you, Joe ______________________________ Joe Woodward Chief Engineer Simulation Support PADT, Inc. www.PADTINC.com 480.813.4884 x156 480.813.4807 fax joe.woodward@padtinc.com Simulation - Product Development - Rapid Prototyping For Your ANSYS Training/Mentoring Needs: https://www.padtinc.com/support/software/training https://www.padtinc.com/support/software/Mentoring CONFIDENTIALITY NOTICE: This e-mail message and any attachments are for the sole use of the intended recipient(s) and may contain confidential and/or privileged information. Unless you are the intended recipient, you are hereby notified that copying, forwarding, printing or otherwise disseminating the information contained in or attached to this e-mail is strictly prohibited. If you are not the intended recipient, please notify the sender by telephone, and immediately and permanently delete and destroy all copies and printouts of this e-mail message and/or attachments. -----Original Message----- From: Bohlen, Dan (GE, US) <dan.bohlen@ge.com> Sent: Thursday, January 18, 2024 7:04 AM To: @EDISON WORKS MECHANICAL_ANALYSIS <EWMA@ge.com> Cc: Zhu, Changming (GE Aerospace, US) <changming.zhu@ge.com>; Perivolarakis, Peter (GE Aerospace, US) <peter.perivolarakis@ge.com> Subject: [Xansys] Crowdsourcing: elastic-plastic model potentially buckling Hi All, Running a an 3D E-P FBO analysis on a military fan shaft. I have a model that ran with a legacy engine set of loads. Run checked out and matches field experience. The same model was run with a new application set of loads that were 50-100% higher and not surprisingly the model crashed at about 60% load. I morphed the shaft to a more robust shape and the model is stopping at 92% load. So I think we might be close to usable design and looking for any tweaks to nudge the solution along. Steps I'm taking: * Rerunning and dumping out results at some substeps before the model diverges to see what's happening. * Trying the STABILIZE command * Tried ARCLEN - didn't help Not sure if mesh size can be an issue (too fine or too coarse). Any thoughts or suggestions welcomed. Charge code=ENG.110264-Y17P Dan Bohlen Senior Engineer, Stress Analysis STAR review chairman, military structures GE Aerospace 1 Neumann Way Evendale, OH 45215 USA Building B90 Column L 3.75 M/D H358 Cell 513-917-3402 Building 200 Desk Phone 3-8816 GE FOCUS: Safety, Quality, Delivery, Cost "In God we trust, all others bring data." W Edwards Deming [IMG_0492]

R

rickfischer51@sbcglobal.net

Thu, Jan 18, 2024 7:11 PM

I second Rod’s comments about your plasticity model. By now you should have a good idea what your max strain is and where its gonna fail. Assuming you have a good material curve, run with a Miso material and take advantage of all the area under the curve up to your max observed strain, then increase tangentially from there. Might get you over the top.

TR

Testi Riccardo

Fri, Jan 19, 2024 8:00 AM

Dear Ms. Bohlen,
Is plasticity the only non linear effect in the model?
Is the solver diverging due to excessive plastic strain increments or to excessive force/displacement convergence values?
Are any geometric singularities present, even in regions you are not interested in knowing the stress state at?
When you examined the situation immediately before divergence, did you see plastic strain and/or displacement values that would justify the adoption of NLGEOM,ON?

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: Bohlen, Dan (GE, US) dan.bohlen@ge.com
Sent: Thursday, January 18, 2024 3:04 PM
To: @EDISON WORKS MECHANICAL_ANALYSIS EWMA@ge.com
Cc: Zhu, Changming (GE Aerospace, US) changming.zhu@ge.com; Perivolarakis, Peter (GE Aerospace, US) peter.perivolarakis@ge.com
Subject: [Xansys] Crowdsourcing: elastic-plastic model potentially buckling

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.

Hi All,

Running a an 3D E-P FBO analysis on a military fan shaft.

I have a model that ran with a legacy engine set of loads. Run checked out and matches field experience. The same model was run with a new application set of loads that were 50-100% higher and not surprisingly the model crashed at about 60% load.

I morphed the shaft to a more robust shape and the model is stopping at 92% load. So I think we might be close to usable design and looking for any tweaks to nudge the solution along.

Steps I'm taking:

Rerunning and dumping out results at some substeps before the model diverges to see what's happening.
Trying the STABILIZE command
Tried ARCLEN - didn't help

Not sure if mesh size can be an issue (too fine or too coarse).

Any thoughts or suggestions welcomed.

Charge code=ENG.110264-Y17P

Dan Bohlen
Senior Engineer, Stress Analysis
STAR review chairman, military structures GE Aerospace
1 Neumann Way
Evendale, OH 45215 USA

Building B90 Column L 3.75
M/D H358 Cell 513-917-3402

Building 200 Desk Phone 3-8816

GE FOCUS: Safety, Quality, Delivery, Cost

"In God we trust, all others bring data." W Edwards Deming

[IMG_0492]

Dear Ms. Bohlen, Is plasticity the only non linear effect in the model? Is the solver diverging due to excessive plastic strain increments or to excessive force/displacement convergence values? Are any geometric singularities present, even in regions you are not interested in knowing the stress state at? When you examined the situation immediately before divergence, did you see plastic strain and/or displacement values that would justify the adoption of NLGEOM,ON? 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: Bohlen, Dan (GE, US) <dan.bohlen@ge.com> Sent: Thursday, January 18, 2024 3:04 PM To: @EDISON WORKS MECHANICAL_ANALYSIS <EWMA@ge.com> Cc: Zhu, Changming (GE Aerospace, US) <changming.zhu@ge.com>; Perivolarakis, Peter (GE Aerospace, US) <peter.perivolarakis@ge.com> Subject: [Xansys] Crowdsourcing: elastic-plastic model potentially buckling 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. Hi All, Running a an 3D E-P FBO analysis on a military fan shaft. I have a model that ran with a legacy engine set of loads. Run checked out and matches field experience. The same model was run with a new application set of loads that were 50-100% higher and not surprisingly the model crashed at about 60% load. I morphed the shaft to a more robust shape and the model is stopping at 92% load. So I think we might be close to usable design and looking for any tweaks to nudge the solution along. Steps I'm taking: * Rerunning and dumping out results at some substeps before the model diverges to see what's happening. * Trying the STABILIZE command * Tried ARCLEN - didn't help Not sure if mesh size can be an issue (too fine or too coarse). Any thoughts or suggestions welcomed. Charge code=ENG.110264-Y17P Dan Bohlen Senior Engineer, Stress Analysis STAR review chairman, military structures GE Aerospace 1 Neumann Way Evendale, OH 45215 USA Building B90 Column L 3.75 M/D H358 Cell 513-917-3402 Building 200 Desk Phone 3-8816 GE FOCUS: Safety, Quality, Delivery, Cost "In God we trust, all others bring data." W Edwards Deming [IMG_0492]