Diving Into Dlubal Part 4: Analysis

Results – The Fruit of Our Labours

At long last, we have arrived at the stage of analysis and design. If you have followed the posts up to this point, you will get to see whether the three-story steel building we created held up. If you want to review our model, you can always return to the previous post for more details. But instead, we have provided a picture here to jog your memory.

Without further ado, let’s get to it. To analyze, we select “Calculate”, “Calculate RFEM Results Only”. During the analysis, there will be a window showing the progress. There is also a dynamic graph showing the maximum displacement for each load case or combination being cycled through.

The analysis is completed in roughly a minute, though it will vary based on the performance of your computer. Analysis times depend on factors such as fineness of mesh elements, overall size of model, number of load cases and combinations, number of iterations specified, and nonlinearities present.

Visualization – Pretty Colours are Meaningless Unless You Know What’s Happening

When your analysis is done, you will first see the deflected shape of the structure in a yellow outline, under the result combination RC1. RC1 reproduces the most critical effects out of all load combinations.

Note that deflections are considered under serviceability limit state so that in general, the deflections produced from the factored load combinations are not considered. Let us look at, for example, the deflection under LC2 – Live Load.

Again, you can see the yellow outline delineating the deflected shape. We would like to make the deflected structure more visible. To do this, we switch to the “Display” tab on the “Project Navigator” tree. Under “Results”, we expand “Deformations”, “Members”, and select “Cross-Sections Colored”. We can now see the deflected shape of the members as coloured contours. The maximum deflection is 13.1 mm from the legend.

Note the deformation scale factor is 320. Let us decrease it to 100 for less exaggeration.

If we also want to hide the original model, we simply go back to the “Display” tab, and under the “Model”, we toggle off “Lines” and “Members”.

Now let us review the critical reaction forces at the origin support. First, we switch the window view back to RC1. We can also toggle off the “Deformation” button in the toolbar to hide the deflected shape for clarity. We switch to the “Nodes – Support Forces” tab in the bottom table after clicking the “Table 4. Results” button, and then click on the origin node. All the reactions for this node (Node No. 1) are now highlighted in yellow within the table. The first two rows show the maximum and minimum values overall for this node out of all the load combinations, then for each case in which the extreme value appears (written in bold), the corresponding values of the other reactions are also given, as well as the associated load combination. As mentioned in the previous posts, this feature is highly useful, allowing users to isolate critical load combinations. In the node selected, when the support experiences maximum compression (min PZ) of -262.95 kN, the load combination which produced that value is CO3 (CO3=1.25LC1+1.5LC2+LC3, where LC1 – Self-Weight, LC2 – Live Load, and LC3 – Snow Load, as previously defined), and the accompanying shear reactions PX and PY are -8.66 and -3.55 kN, respectively. We can also view the reaction forces directly on the model by toggling the “Support Reactions” button in the toolbar.

Let us now look at member internal forces. Say we are interested in strong axis bending of the girders and columns. Under the “Project Navigator” tree, we select “Members”, then toggle on “My” under “Internal Forces”. Because we are in the result combination window, the envelope values are shown. Note that internal forces are expressed in terms of the relative member axes as opposed to global coordinates.

If we wanted to isolate the frame in the X-Z plane along the x-axis, we right click to select “Visibility by Selected Objects”. Now the bending moment envelope is visible only for the first frame.

To get further results for an individual member, say the first girder on the first floor, we can right click on it and choose “Result Diagrams”.

A new window is brought up showing deformations and internal forces along the member length. The current loading case is result combination RC1, though you can select the load case or combination using the drop-down menu at the top. You can toggle on or off the internal forces, deformations, or strains you want plotted. Also, you can hover your cursor over the diagrams and the value at that location will be provided. In the girder we selected, the maximum positive bending moment is 71.22 kN.m while maximum negative is -130.53 kN.m.

To see which load combinations produced these extreme values, we close the window and return to the table at the screen bottom. We select the tab “Members – Internal Forces”, then click on the girder of interest (in this case Member No. 6) to get all the critical internal forces for this member. However, right now bending moment values are shown at regular intervals (0 m, 3 m, 5 m, and 8 m) along the member, and values for the other internal forces are also listed, but we are only interested in the absolute extreme values of My. We can apply filters by clicking on “Result Filter” in the table.

From the dialog, under “Result Combinations”, we can toggle off all options except for “Extreme Values” under “Display:” and select only “My” under “Results max/min of:”.

Once clicking “OK”, and selecting our girder of interest, we can now see that only the absolute extreme values of bending moment of the member are listed and correspond to the ones given in the result diagram, and that both maximum and minimum values appear in load combination CO4 (CO4=1.25LC1+1.5LC2+0.4LC5, where LC1 – Self-Weight, LC2 – Live Load, and LC5 – Wind +x). These rows are highlighted in yellow in the table.

Of course, it is possible to do the exact same thing for the other internal forces as well. For now, though, we will perform design checks for all steel members per standard CSA S16-14.

Was Our Building OK?

First, let us unhide everything by clicking “Cancel Visibility Mode” and toggle off “Show Results” in the toolbar.

Next, we go the “Add-on Modules” menu, and select RF-STEEL CSA.

Once we select RF-STEEL CSA, a new window will be brought up. We click on the “Select Members to Design” button and will be brought back to the model where we can choose the members to design. In our case we will select all steel components.

Under “Existing Load Cases and Combinations”, we scroll down to “RC1” and click “Add Selected Load Case or Combination”. After checking that “Design According to” is “S16-14” is selected, we can click “Calculation”.

Once the calculation is complete, we get the resulting critical design ratios for the chosen members based on the type of check performed (e.g. bending moment, axial, shear, lateral-torsional buckling etc.). In our example, we are interested only in the critical design ratios and not the load combination in which they appear. Under the “Results” section in the list, we select “Design by Cross-Section”, and the table will group the members based on their cross section. We can see right off the bat that some of the members are lacking in design, with a design ratio of 2.07 already visible from the table. Unfortunately, we have some work to do. Clearly, our design will have to be changed (e.g. shortening spans, adding joists, increasing cross-section sizes etc.) to limit the design ratios to 1 or lower.

Let us filter out all members with design ratios higher than 1. We do this by clicking on “Apply Selected Filter to Result Table”, defaulted to show only those members with design ratios greater than 1. Note that some sections are classified as “Non-designable”, which occurs if it is found that, under a specific combination of compression and bending, the section is found to be Class 4 (refer to steel design standards and texts for further information on class of sections).

We find that the highest design ratio is 2.42 for Member No. 13 and click on that row for more information. Under the details table, we can see the step-by-step procedure for determining the parameters to calculate the combined bending-axial resistance, which is the source of inadequacy for this component. The referenced clause numbers from CSA S16-14 are also listed on the side. The format in which the results are presented increases transparency for the users, reducing the so-called “black box syndrome”.

We can also see where in the model our inadequate component is located. We recall that we used W310x60 for the columns. Because of this, let us first isolate only the columns in the model. After closing the RF-STEEL CSA window, under the navigator, we switch to the “Views” tab. Under “Generated”, we check off “Members by Cross-Section” and select W310x60. Now only the columns are shown in the model. Users also have the option to show objects based on other categories, such as material, component type, and geometry.

We now return to the RF-STEEL CSA module. By clicking on the row with the highest design ratio, the member is highlighted in yellow and the critical location along the member is indicated by the arrow.

Checking the Slab – Too Much Stress is Never Good for Anyone or Anything

We will now briefly check the concrete slab for stresses and internal forces. We toggle back on the “Show Results” button so that the “Results” tab is visible in the “Project Navigator” tree. Also, we hide all objects except for the floor slab. Under “Surfaces” and “Stresses”, we select “Equivalent Stresses”, “σeqv,Mises”, and “σeqv,Mises,Max”. The resulting stress distribution is shown.

Note that von Mises stresses are typically applicable for ductile metals and thus have little meaning for brittle materials such as concrete. However, for illustration we will continue to examine the floor slab using Mises equivalent stress. As indicated by the scale on the right, we have a maximum stress of over 1400 MPa! When our concrete is only 30 MPa strong, clearly this means our concrete will fail at the corners even though much of the slab is far below 1400 MPa. Does this mean we will need to make our slab super thick, and if so, how much?

Before we do anything else, let’s visualize the stresses more clearly by changing the scale. To do this, we click on the “Options” button on the bottom right of the legend, and then click on the “Edit Value and Isoband Values” button. A dialog will appear showing the values corresponding to the isobands. In the highest isoband (dark red), we can type in 30, then click “Fill” on the right so all values below will be at equal intervals between 0 and 30.

On clicking “OK”, we can see that stress in much of the slab is less than 30 MPa, but now we can see stress concentrations far exceeding 30 MPa at the columns. It appears our concrete is not strong enough at any of the columns. The reason for the extremely high stresses is because the columns are line members so that their bearing area is concentrated at a very small point, called a singularity. Of course, we cannot take the results to heart because we have a modelling issue as opposed to a structural issue. So how can we take care of this singularity?

Luckily, RFEM gives the option of specifying average regions which distribute stress over a wider area. Say that we want to apply an average area over one corner in one of the openings. The stress distribution prior to averaging is shown as follows.

We switch to the “Data” tab in the “Project Navigator” tree and select “Average Regions”. We select the floor slab as the surface, then choose the node as the centre. The form of our average region will be, say, a rectangle to approximate a baseplate. The dimensions of our region will be a=0.75 m and b=0.75 m, which may be treated as a baseplate close to 30”x30” (quite large compared to the size of columns we have).

On clicking “OK”, our average region is created, and we can see that, over a 0.75 m x 0.75 m area, the stresses have been reduced to below 30 MPa.

For internal forces of the floor slab, we will only review moment along the x-direction, mx, as an example. Returning to the “Results” tab under the project navigator, we will select “Surfaces”, “Internal Forces”, “Basic Internal Forces”, and “mx”. As before, we will change the scale to better visualize moment distribution, by assigning maximum and minimum moments of 20 and -20 kN.m/m.

It is possible to view the extreme moment values on the mesh. We toggle on “Values on Surfaces”, then under “Settings”, we select “Of All Local Extreme Values”, and check off “Minimum”, “Maximum”, and “Show Only Extreme Values”. This will show critical moment values on every mesh node.

However, if we switch to “Of Total Model”, we will only get the maximum and minimum moment values for the whole surface. In our example, maximum and minimum moment both occur at the corners of one of the openings.

As with members, we can also view result diagrams for surfaces. Suppose we want to see the floor slab bending moment in the x-direction along a line passing through the centre of the slab between the two openings. We need to create a section in which to see the bending moment diagram. Under the navigator, we select “Sections”, and in the dialog, we select the points forming the centreline.

We accept all program defaults and ensure that “Show result diagrams in dialog box is checked” under “Options”. Under “Section Name” we give the name “Bending Moment Slab CL”. On clicking “OK”, the result diagram is generated, and we can see the variation of mx along the section length.

After checking the stresses and internal forces for the floor slab, we can use the module RF-CONCRETE to design the reinforcement. Concrete design is more involved than steel and thus will not be covered in this post, which is focused mainly on general analysis and post-processing.


Reporting – Wrapping up Our Findings

Once we have reviewed all results, we can generate our report. In the menu, we go to “File” and “Open Printout Report”.

We continue to click “New Printout Report” and “OK”.

RFEM now generates the printout report. However, we see in the bottom right corner that the report is 791 pages long under the default selection. On examining the contents of the report in the navigator, we can already see that some information, such as nodes, lines, openings, and FE mesh refinements, will not be of interest to our client and we can eliminate them. Suppose we are only interested in loads, reactions, and steel design checks only. We will first get rid of the “Model” category by simply right clicking and selecting “Remove from Printout Report”.

We repeat the process by also deleting the items “Model – General Data” and “FE Mesh Settings”. We are only interested in the critical reactions from the result combination (envelope) and do not need the member internal forces. We can therefore delete “Results – Load Cases, Load Combinations”, and “4.12 Cross-Sections – Internal Forces” under “Results – Result Combinations”. Lastly, under “RF-STEEL CSA” and “CA1 – Design of steel members according to CSA”, we can delete “1.5 Effective Lengths – Members”. Our report is now only 66 pages long, as indicated on the bottom right.

In our critical reactions table, we can see that values from the other result combination, RC2, for serviceability, are also displayed. To disable them, we right click on “4.1 Nodes – Support Forces” and choose “Selection”.

In the dialog, we click on “Select the load combinations to display”, then in the sub-dialog, we select RC2 and transfer it from “To Display” to “Available”.

Now our report only shows the extreme reaction values based on RC1 (ultimate limit state).

Say that now we want to add two pictures in our report: one showing the loading for the Wind +x load case, and another showing deflection due to live load. First, we save the printout report and exit the window. We then switch back to the “LC5 – Wind +x” load case. We also toggle off results and toggle back on the loading and its values. We also switch the view to “View in Y-Direction” to clearly show the wind load being applied (although in 2D).

Next, we go to “File” and “Print Graphic”.

In the dialog brought up, we accept all defaults, but ensure that “Current only” is selected under “Window to Print”.

Once we click “OK”, the report is regenerated to include the picture of Wind +X as seen in the window. The picture is located under “Loads” and “LC5 – Wind +X”. We can save and close the report.

For the live load deflection picture, we return to the main window to hide all loading and show results in the toolbar. In the “Results” tab under the navigator, we toggle off “Members” and “Surfaces”, and toggle on “Global Deformations”. Under the “Display” tab, we deselect “Nodes”, “Lines” and “Members” to hide the original model. For this picture, we want a 3D view and adjust the view accordingly to our liking.

As before, we print the graphic by going to “File” and selecting “Print Graphic”. On verifying all options are correct and clicking “OK”, a message is brought up saying the chapter in which the graphic is to be placed was deleted. From before, we deleted the “Results – Load Cases, Load Combinations” chapter which the picture is to be in. However, this is not a problem as we can recover the chapter only to show the image.

We click “Yes”, and the updated report is generated.

We can see that “4.1 Nodes – Support Forces” has been regenerated despite our getting rid of it earlier. We right click on this to remove from the printout report, and only the live load deflection picture remains. The final report is 68 pages long.

The report may be saved as a PDF. You can also include the name and address of your company. As well, you can save the template of your report for future projects without repeating the process of selecting and deselecting sections.


Reporting is the final step of post-processing and concludes the analysis and design procedure. We have shown you how easy reporting is in RFEM, where we managed to reduce a 791-page report down to less than 70. Design results are very detailed and transparent, making it very clear which parts of our structure we need to fix. Reactions, internal forces, and stresses can all be visualized in an organized manner. Where unrealistic stress concentrations are present, there is even a solution for that as well. Postprocessing within RFEM is as streamlined as preprocessing.

As we have found earlier, we will need to go back to our model and fix our design as the steel components are inadequate. It’s obvious we can’t submit this to our client, and we shouldn’t have generated the report yet. However, when we make changes to our model, the printout report will automatically be updated, including the graphics.

Concluding Thoughts

The three-story steel building from the previous week was analyzed and checked per CSA S16-14 using the RF-STEEL CSA add-on module. We have also walked through basic post-processing steps including viewing internal forces, result diagrams, deflections, and stresses. We discussed briefly on how to handle stress singularities using average regions. Lastly, we touched on how to generate reports, including adding graphics and filtering results.

With this post, we have completed the series on general usage of Dlubal RFEM. The procedures followed throughout are very typical and represent common steps the user will encounter during modelling, analysis, and post processing. Of course, there are many more features in RFEM that have not been discussed, but we believe this series will provide new users excellent reference material for them to develop a solid first understanding of using Dlubal software. As always, please contact ENA2 if you have any questions about Dlubal software!

Wednesday, September 23, 2020

ENA2 CFD Webinar

Tuesday, November 10, 2020

Join us November 18th at 11:00am MST / 1:00pm EST to learn about the different CFD software tools offered by Dassault Systèmes. This blog quickly highlights the three tools we will be going over: FMK...

ENA2 Webinar

Monday, October 26, 2020

Today we'll be talking about how Abaqus can improve your workflow in a 20 minute webinar.

Click here to view all articles.