Sanity check on a steel structure.

LHartley

I have retained an interest in steel structures in retirement (I am not an engineer but worked in construction for many years). I have been experimenting with Mecway and produced the attached model. I wonder if someone could check it out to see if I am on the right track and also I would appreciate any recommendations.

It may be of interest for me to mention that I am running Mecway on MX Linux 19.1 on which I have Wine and Wine Tricks installed. It seems to be running very well.
Cheers

disla

Hi LHartley ,

-You have all the members specified as truss; columns included. ¿Is that ok with you?

-L members have their V axis naturally rotated 45 degrees. That makes you are losing strength capacity of the members and it will be difficult to weld if it isn't corrected. You can change the orientation adjusting the V axis in the element properties window/Rotate by angle.

-I’m sure you know it but for those who are new just point that MECWAY don't check the fulfillment of any Construction Code requirements by itself.
Failure criteria, material safety coefficients, allowable deflection, Load combinations…….. should be check/input by you known the results provided by the software. Some of them can be check automatically with custom formulas. Some others need to be made by hand like slenderness of the members.

-You can try to reproduce some known solutions to start. You will get an idea of how the different elements perform , their limitations and in the meantime, you will get more familiar with the software and how to read the results. See attached pdf. It's in Spanish but you can search for the equivalent in your language.

-Once you are more confident that your results agree with the expected values provided by the theory, you can go and check if the member is suitable to carry that load according to your country Construction Code.

Said that , I wish you enjoy your new journey . I think MECWAY is a perfect tool to start.


Regards

LHartley

Thank you very much for your response disla and for taking the trouble to look at my model.

First step - will change the rotation of the L members but I have another question. Should I set it to 0 or 90?

Second step - I will untick the truss feature for the columns.

Finally thanks for the pdf file. I will look for a similar version written in English.

Regards.

disla

First step - will change the rotation of the L members but I have another question. Should I set it to 0 or 90?

Angle normally would be +/-45º , +/-135º. It aligns the flanges with the Cartesian planes. If you show the beam thickness you can see the final position.

LHartley

Thanks disla - I will post my results maybe tomorrow

Sergio

Hi, @Lhartey , attached a link to a video of a steel tower solved with Code_Aster, the interesting is that the model (step, only lines) is available to download, so you could try to reproduce the results. Mecway will not import the stp, but you can import it in Salome, create groups of elements/nodes, mesh and then import in Mecway.

cwharpe

If you have trouble getting going, here is that file in dxf format. I opened the download-stp file in FreeCAD, highlighted parts, then exported as dxf. In & out, without getting my feet wet.

Verify the scale of the tower. I didn't see anything in the video about spatial dimensions, so I imported the model into Mecway as "mm".

LHartley

@ disla - I struggled with these rotations until I realised I had to be in the "select elements" view - classic newbie lack of understanding I suppose. I think I have it right now.
One thing that is puzzling me is that when I look at the results both the pipeline and structure are coloured except in the case of the reaction results. Is this a glitch in my installation (I am on linux via wine) or is it a setting that needs adjusting?

I am going to try figure out how to put extra nodes in the members and see how that impacts the solution.

@sergio and @cwharpe - that looks quite daunting for someone with my limited skill set but I will have a look at it over the weekend. Thanks for the suggestion.

Victor

Reaction forces are only present at the constraints and their colors are only shown on the corresponding beam end faces.

You can't really refine truss elements because that creates pin-joints at all the new nodes. A way to get a finer mesh is change them to beam elements with flexible joint on beam at the pin-jointed ends and refine them. However, I don't expect it to change the solution unless you have bending of the individual members, such as with gravity or other distributed load.

LHartley

@Victor - thank you for answering my question about the reaction results.
I will explore and experiment with your suggestion about beam elements.

Regards

disla

Hi LHartley,

A must sanity check is to verify that the action/reaction principle is fulfilled.
To check this, create a new named selection for the nodes of interest (I named them Reaction_Force) , recalculate, and then go to Solution/Sum menu to extract the desired parameter. See pict.

If you want to consider the self-weight you need to add a New Gravity in Loads and Constrains and give a density value to each material (See material properties window). It will allow you to compare the structure weight (Tools/Mass =149 Kg) with the vertical Reaction force using the same method descrived above.( Just valid here as there are no other vertical loads)

The L orientation doesn’t look fixed yet and some verticals are still truses . Both options are on the same window. See picture.

I recomend you don't refine beams too much.

cwharpe

@LHartley,

Helps to note Node Order in which elements are first created (eg: to make a mitered picture frame of angles from 4-pts. in a plane, pick nodes (a to b) for each element, say, counterclockwise).

"Invert" element and "Hide All but this" (Component Tree) are also useful tools while you are fixing.

LHartley

Thanks - plenty to keep me occupied and interested here. I’ll post an update next week.

LHartley

@disla - "The L orientation doesn’t look fixed yet and some verticals are still trusses" . I think I have sorted this out now.
I came up with the same "mass" figure as you.
Also followed your instructions about reaction forces after adding a load of 2.5kn each of the four top nodes. I came up with 62.4kn - 31.2kn which if correct means I suspect that each of those bottom two members would buckle.
I presume I am looking for a "failure" solution but I haven't been able to figure that process out as yet.

disla

Hi,

You are progressing very fast.

Be careful. There is a very common mistake. You have applied a TOTAL vertical force of -2.5KN to a “Set of 4 nodes”. That means each node gets -2.5Kn/4 = -0.625 kN.
If you want -2.5KN on each node you need to apply -2.5x4 KN to the SET of nodes or write a -2.5KN load for each node.

Let’s see the reaction sanity check. Magnitude value is a combination of all three directions. It is easier to check each direction separately.

Once fixed the 2.5KN mistake you should get :

Total Vertical reaction on the base (4 nodes)

Action: -2.5KN*4 (force) and -1.445KN (Self Weight) = -11.445 KN
Reaction: 11.445 KN

Action y = - Reaction y (ok)

You can also see the sum of reaction forces at the bottom of the screen.

Buckling check is slightly more advanced. I would first follow the MECWAY Tutorials 2.11 Buckling of a Column.

LHartley

@disla - "Be careful. There is a very common mistake. You have applied a TOTAL vertical force of -2.5KN to a “Set of 4 nodes”. That means each node gets -2.5Kn/4 = -0.625 kN."

I am very glad you pointed that out to me - a dangerous trap!
I think I have it right now although the outcome is marginally different. Can this be ignored?

I will study the tutorial as you suggested.

Regards

cwharpe

@LHartley,

There's nothing like a good project to accelerate the learning curve. Apologies if the following post restates what you already know, but others learning the system may find it useful.

I noticed in the reactions.png file you posted that you Summed Reaction Force Magnitudes for a set of nodes. This generates a caution for the following reasons:

• The Force magnitude at a given node, the calculated scalar from sqrt(Fx^2+Fy^2+Fz^2), tells you nothing about the direction in which it acts. All magnitudes calculate positive, but the force may act positive, negative, or multi-directional.
  
• Even the uni-directional case (one-axis) can be wrong because any negative sense is lost in the calculation.
  
• While force magnitudes can be a useful metric at individual nodes, adding the magnitudes for a set of nodes loses relevance and can falsely describe your system.
  

The tried and true way to find a System resultant Fr for multiple nodes is first find Sum_Fx, Sum_Fy, Sum_Fz. Then calculate the (scalar) Fr = sqrt(Sum_Fx^2+ Sum_Fy^2+Sum_Fz^2). (Resultant direction is calculated using direction cosines.)

I suspect that individual node forces are sufficient in your case, since most Reactions to ground involve connector shear in horizontal plane [sqrt(Fx^2+Fz^2)] and connector tension [-Fy].

LHartley

@cwharpe - I didn’t know that - thank you. - More homework for this week