Plaxis 3D plate output unit kN*m/m

Question

for the output of a plate element unit, I understand in Plaxis 2D, output unit is kN*m/m, that is in/out of plane issue. 
 
 In plaxis 3D, i have a piled protection slab for gas main, the output unit of plate element is still kN*m/m, how do I interpret the total moment, just ignore the /m ? 
 
 M11 and M22 is in 2 different directions of local axis, the plate is very long along the gas main and I don't believe I need to times the length of plate to represent the total moment kN*m. So why the output is shown as kN*m/m

Stefanos Papavasileiou · Accepted Answer

Dear John, 
 The bending moments show the bending of a plate at a location in a certain direction. To get the total bending of a plate in a certain direction, you should make a cross-section at the desired location and integrate the bending moment over its length (not thickness). 
 
 Keeping in mind the simplified Grashoff method would help to understand the units adopted for the forces: 
 this method considers a slab/plate divided into strips of unit width into the two different directions and the forces are thus in the unit of width. Please refer also to the figures below.

Dennis Waterman · Answer

Hi Sonia, 
 This is per foot perpendicular to the cross section. it's a distributed bending moment per meter width.... 
 With kind regards, 
 Dennis Waterman

Renato Reis · Answer

Hi Stefanos, 
 Continuing the discussion I would like to ask you: 
 1) I was checking the Plaxis3D Structural Verification for Plates and Shells (Plates: https://communities.bentley.com/products/geotech-analysis/w/plaxis-soilvision-wiki/45502/bending-of-plates Shells: https://communities.bentley.com/products/geotech-analysis/w/plaxis-soilvision-wiki/45505/performance-of-shell-elements ) and noticed that both verifications consider the plate self-weight as zero. Using the same models I considered the self-weight of the plates and the results were not the same. Using the plate self-weight it was necessary to multiply the max moment by the length of the plate to get the correct value, similar to what you have described. Why this difference? I believe is due to the thickness (d) that I am considering in the plate properties that must be in accordance with the desirable load of the plate. But I would like to confirm this with you. 
 2) I am modelling a vertical tunnel shaft. I am a little bit confused with the discussion about the integration of the results. It is ALWAYS necessary to multiply the moment results by the plate length (perpendicular to the moment)? Or this is applicable only in cases that I want to simplify and turn out the plate into a line? 
 My model is illustrated below. This is only one panel of the shaft. This panel is 5m wide and 50m deep. The M11 value that PLAXIS is illustrating is the final value or do I need to multiply it by the length of the panel? 
 
 3) For the Plates results PLAXIS gives the M11, M11 min and M11 max. How does PLAXIS calculate the M11? 
 Thanks!

Stefanos Papavasileiou · Answer

Dear John, 
 By creating a cross-section of a plate element, you can see the result, e.g. bending moment, along the cross-section length. 
 If you need to find the peak value and location you can use the generated plot, e.g. spotting a local peak value. For getting the bending moment at a specific location of that section indeed you integrate the results over this length. 
 Indeed, in general, the geotechnical engineer needs to sit with the structural engineer and identify the results one needs from another.

Stefanos Papavasileiou · Answer

Dear Mikael, 
 Thank you for the screenshot as it helps understand what you have to deal with. 
 So, in this case, you have a surface plate element with a width of 0.06m and you want to know what is the bending moment at specific locations. The bending moment presented in PLAXIS Output has units of kNm/m because these are the proper units for a surface element, based on the assumptions mentioned before in this post. 
 If you want to assume that this tunnel slice, i.e. 0.06m, is a line element you would integrate the bending moments you see, for instance, when hovering with your mouse using the Hint box (or in a cross-section), over that perpendicular direction. 
 Assuming that the bending moment is constant over the perpendicular direction, you would multiply the value you see with 0.06m in your case, giving units kNm. That would give you an equivalent (assuming constant) bending moment over a 0.06m slice.

Stefanos Papavasileiou · Answer

Dear Mikael, 
 I believe that you have misunderstood my answer and it is important to fully understand what we mean when we integrate the structural forces as this is fundamental when checking the results of your model. It is very critical that you review your extraction of results with a fellow colleague from the geotechnical or (even better) structure team to help you understand this concept of integrating structural forces of surface (plate) elements. 
 To start with, in your original question you asked about integrating the structural forces that PLAXIS gives for a surface plate element to consider/simplify it to a line element. The way to do this is by using the current width of your tunnel slice, which you specified is 0.06m. As I mentioned before, when we do this integration over a slice width, we assume that the results are constant over that width. Then our integration can become a simple multiplication of the result value and the slice width, which in this specific case is 0.06m. 
 The number "0.06m" is no special number but rather refers to the slice width for that specific integration of forces. 
 PLAXIS Output always returns the resulting bending moments in the units of kNm/m as it refers to a surface element and not a line. If one wants to consider simplifying to a line element (from a surface element) an integration of the forces over the width (perpendicular direction to the slice) is required. 
 In your latest post, you mention that you would change the model and the tunnel slice instead of 0.06m would now be 1.00m. The results you will see in Output will still be in the units of kNm/m but if the integration is now done over the 1.00 slice, then that is an easy calculation to make. 
 Note that it is important to understand that the assumption and simplification we make here is that we have a constant result over that width. Therefore, it is not as simple to multiply a width with a value and get a line element out of a surface element. That requires that the considered integration width is much (much) smaller than the full size of the tunnel, for instance, as otherwise, the accuracy of the calculation is far from sufficient. 
 To sum up, I hope that it is now clear that the value of 0.06m is ONLY applicable when you consider an integration over a width of 0.06m and it is NOT a generic number you need to use to consider a line element out of a surface element. 
 Once again, I would strongly advise discussing the way you extract and interpret your structural forces with another geotechnical or structural engineer in case of integrating structural forces of surface elements.

Stefanos Papavasileiou · Answer

Dear Mikael, 
 That is exactly what our Curves manager do. You can select a post-calc node on a plate and plot the bending moment vs. dynamic time. 
 Note that the more steps you have saved, the more detailed the curve plot will be. That is a prerequisite for post-calc points as they depend on the Max number of steps stored setting in the Phases window. 
 Useful read: communities.bentley.com/.../selecting-points-for-curves

Dennis Waterman · Answer

Hi, 
 M11 is based on the stresses that result directly from the calculation. M11min and M11max are just the minimum and maximum value of M11 in the current plot. 
 With kind regards, 
 Dennis Waterman

Dennis Waterman · Answer

Dear Rafi, 
 No, each node has only an M11. M11min and M11max are the lowest and highest value of M11 in the plot, over all the nodes. 
 So if you have a model with 5 nodes with values of M11 of 100,120,90,160 and 110 kNm/m, then M11min = 90 and M11max = 160. 
 With kind regards, 
 Dennis Waterman

Stefanos Papavasileiou · Answer

Dear Nam, 
 As you can see in PLAXIS Output, the plate object comprises of several parts. PLAXIS computes the deformations per element. If you need to consider one value for the whole footing, there is a decision to be made by you as a modeller. Here you can see that part of your footing settles more than the edges. 
 What would then be your single value for a real case as such? As a designer, you should be able to answer that better than any of us.

Plaxis 3D plate output unit kN*m/m

Top Replies