Unexpected extreme deformation values

[Lunamor]

Hey everyone - getting into FEA for a university course and I’m trying to work on my first problem set.

I am analyzing a transmission tower made from 180 T3D2 truss elements.

When applying forces, I see strange deformations at two specific nodes.

This is when adding a gravity load to the structure.

Clearly this is an error of some kind - I would greatly appreciate it, if somebody could point me in the right direction to figuring out what I did wrong here

input file

`*HEADING
Units: mm, N, MPa
*NODE, NSET=Nall
1, 5000.0, 5000.0, 0.0
2, 5000.0, -5000.0, 0.0
3, -5000.0, -5000.0, 0.0
4, -5000.0, 5000.0, 0.0
5, 0.0, 0.0, 5000.0
6, 2500.0, 2500.0, 7000.0
7, 2500.0, -2500.0, 7000.0
8, -2500.0, -2500.0, 7000.0
9, -2500.0, 2500.0, 7000.0
10, 0.0, 2500.0, 5000.0
11, 2500.0, 0.0, 5000.0
12, 0.0, -2500.0, 5000.0
13, -2500.0, 0.0, 5000.0
14, 0.0, 0.0, 10500.0
15, 2000.0, 2000.0, 14000.0
16, 2000.0, -2000.0, 14000.0
17, -2000.0, -2000.0, 14000.0
18, -2000.0, 2000.0, 14000.0
19, 0.0, 2250.0, 10500.0
20, 2250.0, 0.0, 10500.0
21, 0.0, -2250.0, 10500.0
22, -2250.0, 0.0, 10500.0
23, 0.0, 0.0, 17000.0
24, 1500.0, 1500.0, 20000.0
25, 1500.0, -1500.0, 20000.0
26, -1500.0, -1500.0, 20000.0
27, -1500.0, 1500.0, 20000.0
28, 0.0, 1750.0, 17000.0
29, 1750.0, 0.0, 17000.0
30, 0.0, -1750.0, 17000.0
31, -1750.0, 0.0, 17000.0
32, 0.0, 0.0, 21500.0
33, 1250.0, 1250.0, 23000.0
34, 1250.0, -1250.0, 23000.0
35, -1250.0, -1250.0, 23000.0
36, -1250.0, 1250.0, 23000.0
37, 0.0, 1375.0, 21500.0
38, 1375.0, 0.0, 21500.0
39, 0.0, -1375.0, 21500.0
40, -1375.0, 0.0, 21500.0
41, 0.0, 0.0, 30000.0
42, 5000.0, 0.0, 23000.0
43, 4000.0, 0.0, 20000.0
44, 6500.0, 1500.0, 20000.0
45, 6500.0, -1500.0, 20000.0
46, 10000.0, 0.0, 20000.0
47, -5000.0, 0.0, 23000.0
48, -4000.0, 0.0, 20000.0
49, -6500.0, 1500.0, 20000.0
50, -6500.0, -1500.0, 20000.0
51, -10000.0, 0.0, 20000.0

*ELEMENT, TYPE=T3D2, ELSET=Eall
1, 1, 5
2, 2, 5
3, 3, 5
4, 4, 5
5, 1, 6
6, 2, 7
7, 3, 8
8, 4, 9
9, 5, 6
10, 5, 7
11, 5, 8
12, 5, 9
13, 6, 7
14, 7, 8
15, 8, 9
16, 9, 6
17, 1, 10
18, 1, 11
19, 2, 11
20, 2, 12
21, 3, 12
22, 3, 13
23, 4, 10
24, 4, 13
25, 5, 10
26, 5, 11
27, 5, 12
28, 5, 13
29, 6, 10
30, 6, 11
31, 7, 11
32, 7, 12
33, 8, 12
34, 8, 13
35, 9, 10
36, 9, 13
37, 6, 14
38, 7, 14
39, 8, 14
40, 9, 14
41, 6, 15
42, 7, 16
43, 8, 17
44, 9, 18
45, 14, 15
46, 14, 16
47, 14, 17
48, 14, 18
49, 15, 16
50, 16, 17
51, 17, 18
52, 18, 15
53, 6, 19
54, 6, 20
55, 7, 20
56, 7, 21
57, 8, 21
58, 8, 22
59, 9, 19
60, 9, 22
61, 14, 19
62, 14, 20
63, 14, 21
64, 14, 22
65, 15, 19
66, 15, 20
67, 16, 20
68, 16, 21
69, 17, 21
70, 17, 22
71, 18, 19
72, 18, 22
73, 15, 23
74, 16, 23
75, 17, 23
76, 18, 23
77, 15, 24
78, 16, 25
79, 17, 26
80, 18, 27
81, 23, 24
82, 23, 25
83, 23, 26
84, 23, 27
85, 24, 25
86, 25, 26
87, 26, 27
88, 27, 24
89, 15, 28
90, 15, 29
91, 16, 29
92, 16, 30
93, 17, 30
94, 17, 31
95, 18, 28
96, 18, 31
97, 23, 28
98, 23, 29
99, 23, 30
100, 23, 31
101, 24, 28
102, 24, 29
103, 25, 29
104, 25, 30
105, 26, 30
106, 26, 31
107, 27, 28
108, 27, 31
109, 24, 32
110, 25, 32
111, 26, 32
112, 27, 32
113, 24, 33
114, 25, 34
115, 26, 35
116, 27, 36
117, 32, 33
118, 32, 34
119, 32, 35
120, 32, 36
121, 33, 34
122, 34, 35
123, 35, 36
124, 36, 33
125, 24, 37
126, 24, 38
127, 25, 38
128, 25, 39
129, 26, 39
130, 26, 40
131, 27, 37
132, 27, 40
133, 32, 37
134, 32, 38
135, 32, 39
136, 32, 40
137, 33, 37
138, 33, 38
139, 34, 38
140, 34, 39
141, 35, 39
142, 35, 40
143, 36, 37
144, 36, 40
145, 33, 41
146, 34, 41
147, 35, 41
148, 36, 41
149, 33, 42
150, 34, 42
151, 24, 42
152, 25, 42
153, 24, 43
154, 25, 43
155, 44, 43
156, 45, 43
157, 24, 44
158, 25, 45
159, 42, 44
160, 44, 45
161, 45, 42
162, 42, 46
163, 44, 46
164, 45, 46
165, 35, 47
166, 36, 47
167, 26, 47
168, 27, 47
169, 26, 48
170, 27, 48
171, 49, 48
172, 50, 48
173, 26, 50
174, 27, 49
175, 47, 49
176, 49, 50
177, 50, 47
178, 47, 51
179, 49, 51
180, 50, 51

*BOUNDARY
1, 1, 3
2, 1, 3
3, 1, 3
4, 1, 3
*MATERIAL,NAME=EL
*ELASTIC
70000.00, 0.3
*SOLID SECTION,ELSET=Eall,MATERIAL=EL
2500.0
*STEP
*STATIC
*CLOAD
1,3,1043.01
2,3,1043.01
3,3,1043.01
4,3,1043.01
5,3,2015.96
6,3,1620.17
7,3,1620.17
8,3,1620.17
9,3,1620.17
10,3,791.40
11,3,791.40
12,3,791.40
13,3,791.40
14,3,1552.79
15,3,1490.11
16,3,1490.11
17,3,1490.11
18,3,1490.11
19,3,627.23
20,3,627.23
21,3,627.23
22,3,627.23
23,3,1264.40
24,3,1492.36
25,3,1492.36
26,3,1492.36
27,3,1492.36
28,3,519.98
29,3,519.98
30,3,519.98
31,3,519.98
32,3,833.21
33,3,841.79
34,3,841.79
35,3,841.79
36,3,841.79
37,3,315.80
38,3,315.80
39,3,315.80
40,3,315.80
41,3,956.15
42,3,1019.10
43,3,386.11
44,3,609.12
45,3,609.12
46,3,445.20
47,3,1019.10
48,3,386.11
49,3,609.12
50,3,609.12
51,3,445.20
*NODE PRINT,NSET=Nall
U, RF
*EL PRINT,ELSET=Eall
S
*NODE FILE, OUTPUT=3D
U
*EL FILE
S
*END STEP `

edit: nodes 43 and 48 are the strange ones

[JuanP74]

your design is faulty. At least three non co-planar trusses have to converge at each node

[Lunamor]

I see, thank you very much.

I suppose this is what the prof wants to teach with “If needed, additional elements are to be added, justify each addition”

You did this visualization in cgx, may I ask which commands you used?

I can’t quite figure out the documentation around plot

[JuanP74]

plus n all r
seta nodes n 43 48
plus na nodes b

[Lunamor]

thank you again!

I hope another question isn’t too much, considering you already helped me out a ton.

Am I right to assume, that the reason for the error, then, is that nodes #43 and #48 are unable to deal with any forces in the z direction?

calculix mentions, regarding the truss elements, that they cannot sustain bending. That’s what I would correlate with forces in the z direction.

When calculix then tries to apply the load I set, in the original structure, there is simply no resistance to those nodes moving to infinity. Even though, as soon as the trusses are moved slightly, they would experience strain and therefore counteract that displacement. But there is only one calculation step with how the input file is set up. Also, the direction in which they can move is undefined at the start, so they could shoot up or down (which my original picture shows nicely).

[JuanP74]

mathematically you are solving K*U=P so if the stiffness is zero, and the load is finite, there is no solution, that is K is said to be singular->not a structure but a mechanism. Commercial softwares would say K is singular so no solution, but calculix tries to provide a hint on how the mechanism would move, that’s what you see, the sign is not very relevant. From a physical point of view you have spherical joints at any joint in the truss, and members only can take axial load so until it deforms (a lot) vertical load can’t be taken, but this is a nonlinear behaviour and you did a linear analysis so no chance of seeing this behaviour. If you try to add the NLGEOM parameter to the STEP card you’ll see it tries to balance that load but other issues arise.
I’d recommend revisiting the theory, e.g.: https://eng.libretexts.org/Bookshelves/Mechanical_Engineering/Introduction_to_Aerospace_Structures_and_Materials_(Alderliesten)/02%3A_Analysis_of_Statically_Determinate_Structures/05%3A_Internal_Forces_in_Plane_Trusses/5.03%3A_Determinacy_and_Stability_of_Trusses

[Disla]

Seems Victor has just identified the issue. It could to be related with the same elements included in both element sets at the same time. He is working to clean it.

[Lunamor]

Thank you Juan! Indeed theory is similarly lacking as practical application in my case.

Though it’s less the fundamental technical mechanics and more the jump to numerical solutions and how the codes work specifically.

I just started the course and while I think the subject matter is extremely interesting, my professor is not very helpful.

Thanks for pointing me in the right direction!

As for Dislas original post, the gravity indeed points in the wrong direction, thanks for catching that!

I used *dload with GRAV before, but switched to this after I encountered the problem the first time.

Once the model works correctly, I’ll probably revisit that to see if the results are the same. I don’t fully understand how that command card works yet, so baby steps.

[Disla]

It’s a good practice to always check reaction forces are in balance and perform a preliminary frequency analisys (It’s very fast) to be sure all your memebers are properly connected and there are not rigid body modes.
Good luck!!

[JuanP74]

Always blame the system, not the teacher!
May the force (and the resulting displacements, according your stiffness) be with you.

[xyont]

it should be not really a problem when there’s no out of plane force for the truss element or adding required member to transmit. In a rare situation, without an additional member, the truss maybe changes to beam element to resist bending.

free vibration analysis based on mass source from truss member selfweight only will detect some problem due to mechanism. However, this actually not true since in reality truss member still have some rotational end restraint. Significant lumped mass from another source also will reduce the actual problem in vibration modes.

[Disla]

@xyont

it should be not really a problem when there’s no out of plane force for the truss element

Of course, if gravity gives us problems, we eliminate it. Why didn’t I think of that before?

[xyont]

simple explained, truss element with both end pinned connection is no more than just assumption which physically does not exist. It may still okay for it’s self weight due to gravity loads or out of plane self mass inertia movement.

many physically build exist such as X braces at bridge floor (gravity cases) or these type bracing in building frames (inertia cases) to resist lateral loads of wind or seismic. Too simple in model with truss element, small deformation, ignoring end rotational stiffness, etc can not explain this proofed condition.

[Disla]

Midspan nodes on a truss element doesn’t have any sense to me.
I would (I did) suggest a one piece truss before removing loads or adding new members.

[xyont]

if that’s problem only a homework, all suggestion are freely to decide based on personal sense. In case of real project and needed to build, i will suggest at least two (as shown before) to six additional member in models. This decision can be known after all gravity and lateral loads has been considered in analysis and design of the member itself.

[Lunamor]

Thanks everyone! I’ll probably add in that extra truss and call it a day.

[xyont]

indeed, these X brace configuration of truss member can be solver problematic at out-of-plane deflection even for small amount of force due to self weight case, but physical reality says not.

below simple example case solved by OOFEM & CalculiX solver which shown result is way of. An experience did not fully trust the result, the weight and mass of these truss members will be excluded and ignores in analysis. Equivalent nodal loads or mass are assigned to corner nodes directly.

[JuanP74]

that’s not a trusswork structure but a bending 3D frame

[xyont]

my example is a sub-model of brace member similar to truss element, only transmit axial force. Bending is in beams and column at global models, it does not really affect the sub-model since displacement only fixed (no rotational).

take sub-model of space truss like tower structure as original post, it could be similar problem in self weight by the solver. In practice, i do simple ignore by excluding, replace with another equivalent since in physical reality shown not a problem.

[xyont]

always interesting to conduct full three-dimensional analysis to explain clearly about the condition, result shown not a problem due to selweight. Deflection about several millimeters only and it seems to be consistent with physical reality, not in few meter as previously of truss model by OOFEM solver or almost infinity by CalculiX solver.