Skip to main content

Weld Analysis with Ansys

Figure 1: Equivalent Stress of White Paper Model

There are many software out there now that does weld analysis. Among others...
  • For fatigue type analysis, there are: FE-Safe (Verity Method) & Ncode (Volvo Method)
  • For static type analysis, there are: FEWeld & EDRMedeso

A good reference classic book is Blodgett's Design of Welded Structures (1966). This book is a real gem even though it's quite old.  Here is a short write-up by the same author et al with similar material: Welded Connections.

White Paper
Figure 2: Weaver's White Paper Comparing  FEA to Hand Calculations

I came across this really good white paper by Weaver Engineering that had a worked example comparing both hand calculation to their software along with in depth discussions. The example was detailed enough to be replicated. This is a great stepping stone when following the crawl-walk-run philosophy.

The rest of the post seeks to replicate the results in the white paper.

Model and Snippet Comments
A critical step in setting up the model is highlighted in Figure 3. Nodal Forces has to be computed for later post processing and "Save MAPDL db" is required for later named selection pointing. This should be done before the model is solved.

Figure 3: Key Settings

Secondly, the forces at the weld-line was extracted with the elements of the terminating member selected. As noted in the FSUM help document: "Sums and prints, in each component direction for the total selected node set, the nodal force and moment contributions of the selected elements attached to the node set." To find the "effective length" of the weld associated with the extracted load, the average length was taken (see script for details).

Finally, the Workbench model takes advantage of Ansys DesignXplorer with Snippets similar to a previous post to test the sensitivity of mesh size.

Figure 4: Ansys Results with Different Mesh Density

In Figure 2 by Weaver, his peak weld force/length (fw) from hand calculation comes in at 2,390lbf/in. In this Ansys Model and associated script, it peaked at 2,775lbf/in for 10 elements along the weld line (WELDFORCE10.txt). As the number of elements is increased, so too did the force/length. It appears to be a singularity there though the good news is that if one is to use the "hot spot method", the trend is slightly under 3,000lbf/in which is in line with the White Paper's FEA model.

A better way of averaging out the forces at the end could be finessed if needed. All the best!  

Source Files
  • Archived Ansys Workbench File V18.2:  Link
  • APDL Snippet Used in Ansys Workbench: Link
  • Octave/Matlab Plot Script: Link


Post a Comment

Popular posts from this blog

ANSYS User Defined Results

There is an abundant of options in ANSYS classic when one wishes to post process results. ANSYS workbench default pull down menu post processing options are more limited but they can still be accessed via the User Defined Results. One way not commonly used but can come in handy is as follows: Zeroth: Under Analysis Settings, there is "Output Controls" where you can toggle to "Yes" what you would like to save before the solution starts. This is like OUTRES in APDL. Output Controls First: After solving the model, click on Solution in the tree to highlight it. Solution Second: Click on Worksheet in the toolbar. Worksheet Third: In the worksheet, you will see list of results that are saved. Right click on it to create the User Defined Results. Create User Defined Results So here we have it. You could of look up the different expressions in the help document but I find this method of accessing the results convenient.  Example: Aspec

Export Stiffness Matrix from Ansys

It is sometimes useful to extract the mass and stiffness matrix from Ansys.     *SMAT, MatK, D, IMPORT, FULL, file.full, STIFF       *PRINT, matk, matk, txt Exporting mass matrix would be similar:       *SMAT, MatM, D, import, full, file.full, MASS The above script uses APDL Math to get the job done. (Please see previous post for another example). The ordering of the matrix is unfortunately not concurrently exported. To verify the sequencing is as expected, we will work to replicate a truss example in the  Finite Element Trusses course notes by Bob Greenlee. Figure 1: Truss Problem Setup Model Creation Script to create model: /prep7 !! Creates Model to reflect course notes ! Properties et ,1,1  mp , ex, 1, 29.5e6 r , 1, 1 ! Geometry n ,1 $  n ,2, 40 $  n ,3, 40, 30 $  n ,4, 0, 30 e ,1,2 $  e ,2,3 $  e ,1,3 $  e ,3,4 ! Boundary Conditions d ,1,ux,0 $  d ,1,uy,0 d ,2,uy,0 d ,4,ux,0 $  d ,4,uy,0 f ,2,fx,20e3 f ,3,fy,-25e3 ! solves /solu eqslv , sparse

ANSYS APDL Syntax Highlighting editor

Notepad++ with APDL User Defined Language The editor of my choice is Notepad++  with the available User Defined Language Files for APDL . You can install it without administrative privileges via the zip file. The best part of it is, it's FREE! After installing Notepad++, go to "Language>Define Your Language..." then "Import" the XML file downloaded from the above link. Remember to restart Notepad++ so that the language changes will take into effect. Opening up any *.inp or *.ans files should automatically switch highlighting to APDL. I made some minor edits. Here's my XML file: LINK . I also heard Sublime Text and  Ultraedit  has more advance features but they aren't (totally) free.