Strand 7. Simple case with the warning of Node force/moment component at node X is ignored.

[Norahh]

Hi guys!

I have a problem about the beam I am analyzing. I should do a nonlinear analysis, but there are always warnings and all the displacements are zero. So I thought I did a linear static analysis first to see what went wrong. And this warning came, the Node force/moment component at node 1 is ignored, node 1 is where the force is applied. And the displacements are all zero. The horizontal beam was simply supported, to the right there is a vertical beam connected to the horizontal beam with both ends fixed.

Can anyone tell me how to fix this problem please?

Many thanks.

 

[IDS]

Norah - if you upload the st7 file I will have a look. Also an image showing the beam arrangement and load and boundary conditions would be useful for those who don't have Strand7.

At the moment all I can suggest is checking that your global freedom conditions are OK, and that the applied load(s) are not applied at a restrained node.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Norahh]

IDS- Thank you so much. I attached the strand 7 file. I set the global freedom case as 2D beam. According to your reply, I should not apply the load to the left hand side node that I did now. But then how to apply the load?

 

[Norahh]

Also this is the image of the beam.

 

[Norahh]

Almost forgot. The property of the beam is just a random choice from the library.

 

[Norahh]

And the horizontal beam has an imperfection in the shape of sinus. In order to simulate this, the beam was replaced by three beam elements.

 

[IDS]

Do the restraints you have used represent the actual structure? Nodes 1 and 4 are rigidly supported for displacement, but are free to rotate, except node 4 also has the two beams that will restrain rotation?

If so any load applied at Node 1 will go straight into the support, and will not affect the rest of the structure, which is what your analysis found.

To get some load into the structure either apply the load at one of the unrestrained nodes, apply a moment at Node 1, or remove one or more restraints at Node 1.

It just depends what you are trying to model.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Norahh]

IDS-Thanks a lot. I freed the restraint of x direction of node 1, then it worked fine. I tried to conduct nonlinear analysis, set the value of force 100 kN, changed the property of beam to the question asked. After reading the examples of help of strand 7, I created a stress vs strain table, then set the load increment from 0 to 3. And the results were weird, all the displacements were zero. Could you tell me what went wrong? I am sorry for lots of questions, I am new to strand 7, especially the nonlinear part. I have attached the new file.

 

[IDS]

Your first increment result has zero stress and deflection because the load factor was zero.

To view the other increments open the results file and click on the increment dropdown box in the top-left corner.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Norahh]

IDS-Thanks. This question was so stupid. I get it now.
Can I ask another question if it is not bothering you The thing is: I tried to delete the stress vs strain table, and then the results turned out to be better (no warnings or notes), so I guess it is okay to delete the table, right? And for the results, I drawn the displacement of node vs load factor plot, there was no drop, i.e. no buckling. I wanted to plot the displacement of the centre of the horizontal beam vs load factor, but there was no node at the centre. Hence, I plotted the curve of node 2. Sorry I am a little chatty, anyway, my question is how to plot the curve of the displacement of centre vs load factor and how come there was no buckling? Thanks again.

 

[Norahh]

I increased the load factor and there was a drop. So it seemed that I found the problem.

 

[IDS]

Norah - don't be worried about basic questions, but you do need to think about what you are modelling and make sure your computer model is a reasonable approximation to it.

In general you should only be applying restraints in the model if the actual structure has something preventing movement (or rotation) in that direction.

If you are looking for buckling loads the vertical restraint you have at node 1 will make a big difference. Is the actual structure restrained vertically at that point?

Also does the other end of the horizontal beam have restraints other than the two vertical beams?

Are the top and bottom of the vertical beams effectively restrained against rotation, or just in position?

Regarding the stress-strain table, if your beam is still in the elastic range when it reaches its buckling load then you don't need a stress-strain table, but if the stress anywhere is approaching yield you will need it. The simplest thing to do is to do a run with and without (making sure that non-linear material is enabled), and see if it makes a difference.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Norahh]

IDS-Thanks for your reply. The end of the horizontal beam has restraints other than the two vertical beams, the top and bottom of the vertical beams are restrained against rotation and position. And I wanted to plot the displacement of the centre of the horizontal beam vs load factor, how can I do it without subdividing the centre element into two elements?

Thanks again, I have been learned a lot from you.

 

[IDS]

And I wanted to plot the displacement of the centre of the horizontal beam vs load factor, how can I do it without subdividing the centre element into two elements?

The easiest way is to subdivide the beam so you have a node wherever you want deflections.

Alternatively, open the results and either:
Click on the results settings icon (multicoulered icon)
Set number of slices to an odd number
Open result listings
Click beam tab
Select "Beam Stations" from the View drop-down box
You will now have displacements listed at points along each beam, including the mid point.

Or

Click the "peek" icon (microscope)
Click the beam tab
Set slices to 3
Select displacements
You will now get displacements at each end and the mid-point when you click on any beam.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Norahh]

IDS-Thank you so much. Here is another question, hope you can help. I want to use displacement control method, how can I do it? I checked the master-slave link in the help, but I didn't really get it.

 

[IDS]

When you define a node restraint the default deflection is zero, but you can enter a non=zero deflection in any direction.

You can create separate freedom cases with different node deflections (see the Global menu).

To gradually increase the deflection run a non-linear static analysis, create as many load increments as you need and apply factors to the Freedom Case.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Norahh]

IDS-Thank you so much. Sorry for the late reply, there is no email reminding this time. I have managed to conduct displacement control method in several other models. Some of them the master-slave link was used.