Modal Analysis of Plate using lines and beam elements

[kylehudson]

ANSYS Help: Simple Modal Analysis of Plate

I am modeling a plate (36"x3"x.25") in ANSYS. When I construct a line out of two keypoints and give the line a rectangular section, the analysis works and I can output modal displacements just fine. With these modal displacements I can plot the mode shapes outside of ANSYS. I can also see the mode shapes animated inside ANSYS.

However, if I try to construct the same plate using the same section out of 4 key points (2 long lines and one very short one in between) I get bad results. When I output my modal displacements for the each mode I see a huge spike at the in-between key points.

Its like there is a discontinuity between the key points or lines in the middle, even though all my lines' section properties are the same. When I plot my node numbers, I see that ANSYS has moved my node at the in-between line to the last point of the next line. Therefore, that node's displacement is huge relative to where its location is supposed to be.

(I.e. ANSYS has taken node 65, which is at the middle of my in-between line and moved it to after node 315, the last node of my line. Node 65 now sees a displacement that node 316 would, not node 65)

I am using beam189 elements with an element size of .4mm.

ANY HELP WOULD BE APPRECIATED

 

[minger]

I'm not sure why you would try and use 4 keypoints, and not sure what you're attempting to accomplish by doing so. With your l/D ratio, you are situated very nicely in the realm of simple beams.

Keep it simple for what you're doing; the two KP approach is fine for the time being. If you need additional nodes "inside" the beam, I believe you can specify the number of nodes using the SECDATA command when you define the cross-section.

 

[FredGarvin]

I agree with Minger. The addition of a very short, i.e. stiff member doesn't make a whole lot of sense to me. If you wanted to increase the fidelity of the mode shapes (sensitivity analysis), you can play with modifying the mesh, but I don't understand the addition of more elements.

 

[nvn]

kylehudson: I would think you can define any number of keypoints you prefer, and it should work fine. Therefore, on a temporary copy of your model having four keypoints, delete the solution results, then move the middle keypoints, say, 20 mm in different directions perpendicular to your current straight line. See if any lines are connected to the wrong keypoints. If not, delete a line, and see if there is another coincident line underneath it. Also, delete a keypoint, and see if there is a coincident keypoint underneath it. In other words, check the model for coincident lines, lines connected to the wrong keypoints, disconnected lines, coincident keypoints, and coincident nodes. If no problem is uncovered, try deleting and recreating the model. Or try creating a new model again, and see if it exhibits the same problem. Let us know what you find.

 

[minger]

When you mesh a line with beam elements you get essentially a self-contained beam (for lack of a better word). So, if you're trying to analyze a single beam, then you use a single line, with two keypoints, more if you need them for any reason.

When you have two parallel lines connected by another line, it doesn't matter what your node pattern looks like, the solver is computing the solution as if you have two separate beams connected in the middle by another beam.

Use:

/ESHAPE,1

To turn on element shaping to see exactly what the solver is solving. With rectangular cross-sections, you can increase the fidelity by one of two ways.

- Increase the number of cross-sectional points by SECDATA

- Increase the mesh density by issuing a LESIZE,elem_size prior to LMESH.

 

[kylehudson]

Thanks for the responses. I am introducing more key points into my beam because I want to give that small intermediate line different section properties than the rest of the beam. I.E., I want to have damage in my beam, but I want the beam to act as a whole.

For instance for the undamaged part of the beam, I will have a section of thickness, say .25", then for the very small intermediate line, I am giving it a thickness of say .15 inches.

This solution converged and I was able to read the nodal displacements and a spike showed up in my modes. I thought this was indicative of the damage (less thickness) but in reality it was indicative of the fact that ANSYS has moved my nodes around. As shown in the pictures, node 316 is moved to the end of the beam, even though it should be at my small intermediate line. Therefore it sees the displacement of node 470. This produces a large spike.

To test this, I created the beam with 2 long lines and 1 intermediate short line. I gave them all the same section properties and sure enough a spike showed up in the nodal displacements, not because of damage but because ANSYS has moved the nodes

 

[minger]

Can you show your input file? I'd like to see exactly how you're doing this.

 

[kylehudson]

I used GUI so its going to be messy. Attached.

 

[minger]

You're completely right; that is a ***** to read. From what it seems like, you should be able to do something like:

/PREP7

damage_depth = 0.010
beam_length   = 36.0
beam_width   = 3.0
beam_height  = 0.25
damage_loc   = 18.0
damage_width = 1.0
elem_size = 0.10

!--material properties here

ET,1,189
refine = 1  !--beam refine parameter
SECNUM,1
SECTYPE,1,BEAM,RECT,normal,refine
SECDATA,beam_width,beam_height,nodes_width,nodes_height
SECOFFSET,CENTROID

SECNUM,2
SECTYPE,1,BEAM,RECT,damage,refine
SECDATA,beam_width,beam_height-damage_depth,nodes_width,nodes_height
SECOFFSET,CENTROID

k,1,0,0,0
k,2,beam_length-damage_loc-(damage_width/2),0,0
k,3,beam_length-damage_loc+(damage_width/2),0,0
K,4,beam_length

*DO,i,1,3
L,i,i+1
*END DO

LESIZE,ALL,elem_size
SECN,1
LMESH,1
LMESH,3
SECN,2
LMESH,2

Or am I missing something?

 

[kylehudson]

I ran your code and added material properties. When I ran it just as you have with no section given to the small line, the mode shapes of the left long line act completely independent of the mode shapes of the right long line. The first pic i attached shows that.

Then I gave the same section that the long lines have to the short line. I did the modal analysis, and plotted the modal displacements. Just like my results, there is a huge spike where you have the small line in the middle, even though the beam has no irregularities as far as size/properties. The second pic shows this.

However, when I rearrange the nodal displacements (move nodes 703-721 to in between 351 and 352, as ANSYS has numbered it on the third pic), the nodal displacements are correct and give a good mode.

So I guess this is a numbering issue. I either need ANSYS to output nodal displacements in order of their actual location, or I need to renumber then nodes on our beam so that regardless of how many lines, ANSYS shows 1-700 in the correct order. Is this possible?

 

[nvn]

kylehudson: I'm not yet convinced you have checked your model for coincident, disconnected keypoints and nodes. See post 4. And/or issue the command nummrg,kp, or nummrg,all.

Next, perform a modal analysis, and display the mode shapes (displacement) of your structure. If you see any elements on your screen that are disconnected, then it means your model is still not constructed properly, and your beam elements are still disconnected. If so, continue working on your model until you get the disconnected elements connected together properly. Don't even worry about drawing a graph until you get your elements connected together. Let us know if it still fails.

 

[minger]

No, the node numbers shouldn't matter what order they are in. They are just in that order because of the way we meshed them.

If you want them in more numeric order, you can mesh the lines sequentially, but you'll need to make sure to switch SECNs.

If you think that the geometry is disconnected, you can issue a NUMMRG command after meshing which will merge anything coincedent. (NUMMRG,ALL, will merge keypoints, nodes, elements, element types, materials maybe, etc etc). Note that for merging keypoints, you will need to define a tolerance value.