How to modify parts section

[Anonymous]

Hello dear guys

I am beginner in Simulation Mechanical. I am going to do random vibration analysis on a structure. I modeled a structure in robot structural analysis, and since as far as I know there is no option for random vibration analysis in Robot, I need to do it in Simulation Mechanical. I save the model as DWG file and opened it in Simulation Mechanical, but in the first step, I do not know how to group the elements with similar sections. Because as far as I know, for each group we can assign only one section. On the other hand, as a default three groups have been created for my model,  and I select "Beam" as the element type, but when I click on edit element definition, it doesn't work and gives me an error saying that "the part does not contain valid geometry". I attached my DWG file. It is kindly appreciated if somebody can help me. Thank u so much in advance

Regards

[marwan_azzam]

Hello Mojtaba,

I am going to guess the reason it says "the part does not contain valid geometry" is because all your lines are construction lines and not actual lines.

If all the lines appear in color black then they are construction lines.

What you need to do is:

1- Go to Selection: Construction Objects

2- Select all the construction lines

3- Right-click and choose Edit Attributes

4- Uncheck "Construction object"

As far as beam cross sections, any given part (or group) if assigned beam element type can in fact have more than one cross section.  Lines on different  on different layers can have different cross sections.

You can change the Part, Surface, and Layer attributes by:

1- Go to Selection: Lines

2- Select lines of interest

3- Right-click and choose Edit Attributes

4- Change the Part, Surface, Or Layer number.

Alternatively, of course, you can also group them on different parts by following the 4 steps above.

If you need further assistance please let us know and if need be create and attach the archive file of your Simulation Mechanical model.

[Anonymous · Accepted solution]

Thank u so much for your response and great explanations. I followed your steps and it worked for me. I created several parts and assigned the components with same section to each part.

For the next step, I am going to assign boundary conditions and do natural frequency (modal) analysis and then random vibration analysis to identify the vulnerable and critical components.

But I have two questions before going to the next steps:

1. Am I be able to generate mesh for the beam components?

2. Am I be able to put boundary conditions under the structure in any location. As far as I know, I can only select a line and then assign boundary condition under that line, then the supports will be automatically assigned. I cannot put supports in any location by clicking on them like other softwares.

Thank u so much again.

[marwan_azzam · Accepted solution]

Hello Mojtaba,

I'm glad my post was helpful.

Please mark it as a solution when you get a minute.

As for your other two questions:

1- You really cannot "mesh" beam elements per se. What you do is divide them into multiple elements.  To do that:

  a- Go to Selection: Select: Lines

  b- Select the beams you want to divide

  c- Right-click and choose Divide

  d- Enter the number of divisions and hit OK

2- Assigning constraints to beam elements has to be done on nodes not lines.

  a- Go to Selection: Select: Vertices

  b- Select the vertices to which you want to apply constraint

  c- Right-click and  add the boundary conditions

Number 1 above ties into number 2 in that you want to divide the lines in such a way to obtain the nodal locations to which you want to apply the constraint

Please let us know if you have further questions.

[Anonymous]

Dear Marwan

Thank u so much for all your helps and guidances. I followed all steps you explained. I assigned  sections to each part of my structure. I divided each line and assigned  hinge support to my structure. But when I want to do natural frequency (modal) analysis before random vibration analysis it doesn't work. I don't know why. I tried to attach my file here but it said that the file with (fem) format does not have a valid extension for an attachment and has been removed. Is there any other way to send my file directly to you to look at and check my file? Thank u so much

Best Regards

Mojtaba

[John_Holtz · Accepted solution]

Hi @Anonymous.

The .FEM file is not the complete input, so that is why you cannot attach it to a post.

You want to create an archive ("app button > Archive > Create") and attach it to your post. Alternatively, you might want to explain what happens when "it does not work"; the problem could be something with your computer instead of something wrong with the model.

[Anonymous]

Thank you John for your quick response

Yes. You were right. I closed the software and reopened it and it worked. But I have another problem. Before I do random vibration analysis, when I do natural frequency (modal) analysis, I see that the results are wrong. The Modal Effective Mass in X, Y, and Z direction are %0.22, %0 and %0 (which must be more than %80), and also the frequency is not correct ( e.g. the first one is 8.2733E-07 cycles/sec). Do you know what I should do to correct it? I saved my file as archive file and attached it here. Thank you so much again for your time

[John_Holtz · Accepted solution]

Hi @Anonymous

The results are "wrong" because the model is wrong. A zero frequency result implies that the model has rigid body modes. When I view the results and exaggerate the displacement ("Results Contours > Show Displaced > Displaced Options"), I can see 5 members that are obviously not connected to the rest of the frame. See the attached image "unconnected beams.png". It looks like there are many other beams that are not connected together.

Since your model does not have any constraints in the three translation directions, there will be three rigid body models. (You only have the three rotation directions constrained.) So, solving for five modes may not be enough to get the 80% mass participation that you want. You should edit the Analysis Parameters and specify many more modes. (10? 20?)

In order for beam elements to be connected together, they need to share the same node. For example, the vertical members need to be intersected ("Draw > Modify > Intersect") where beams 1, 2, 3, 4 cross. After intersecting the lines, you may need to snap the model together ("Draw > Modify > Set Search Tolerance" and "Global Snap").

The attached image was created with the elements shrunk ("Results Options > Shrink Elements"), so the gap between the lines show where the nodes are located. Any location where the end of a member meets at a node is connected. Any place where the end of a member meets on a line segment is not connected together.

For future reference, the workflow should have been something like this:

1. Split the lines in the native document where they meet, or
2. Intersect the lines after importing into Simulation Mechanical.
3. Create the mesh on each line segment. If the lines are construction lines, you can use "Mesh > Structured Mesh > Divide 1 Object", or convert the construction lines to regular lines and then divide them.

You are close to having an answer! One last iteration should do it.

[Anonymous]

Thank u so much John for your helps

I defined  constraints in the three translation directions (hinge supports). Then I tried to connects the lines. First I had some problems. I went to draw -> Intersection. Then I selected the lines which are intersected to each other as shown in the attached pics, but it didn't work for some of them. Finally after trying several times it worked I think. But the issue here is that it is still wrong I think. I increased the number of frequency to 20. Now the effective mass in X direction is 54.7% (which should be less than 80%), in Y direction is 94.36% and in Z direction is 81.37%. The frequency is still too small (for the first mode is 0.17 cycles/s, and for mode 20 is 2.7 cycles/s). I attached my model again. Could u please look at my model. Thank u so much

[John_Holtz]

Hi @Anonymous

I agree that all of the members are connected together now. That's good. 

As for the modal results, my guess is that there is something wrong with the constraints. It seems like a rather large structure (36 m x 12 m x 16 m) to be held by 2 points (plus some other points with only rotation constraints).

As a "hand calculation", I applied gravity in the Y direction and performed a linear static stress analysis. The structure displaced 10.1 m in a shape that is similar to the mode 1 shape. This displacement is very large, so that implies that something is wrong (either the constraints, materials, beam cross-section, or orientation.)

But assuming the displacement is correct, the natural frequency can be estimated from the stiffness of the structure and mass. Based on the calculated weight of 3.6E5 N, the stiffness of the structure is k = W/d = 3.6E5/10.1 = 35.6E3 N/m. Then frequency = sqrt(k/m) =sqrt(k/(W/g)) = sqrt(35.6E3/(3.6E5/9.81)) = 0.985 rad/sec = 0.157 Hz. This is close to the value that Sim Mech calculated (0.174 Hz).

Does this provide any clues to what is going on in the analysis?

[Anonymous]

Thank you so much John for your explanation.

I reduced the size of module to 36 ft(Length) x 12 ft(Width) x 16 ft( Height) to make it  smaller. I exactly followed the previous steps and defined everything correctly. I made all supports fixed and did natural frequency (modal) analysis again. I used 30 frequency. This time it gave me more logical value for frequencies ( 9.73 cycles/sec in mode 1 and  20.8 cycles/s in mode 30), but unfortunately it gave me wrong modal effective mass especially in Z direction. modal effective mass in X direction is 50.68% (should be more than 80%), in Y direction is 61.74% (should be more than 80%) and in Z direction is 0.124 which is completely wrong. I attached my file again. It is kindly appreciated if you can check my new file again to see what the problem may be. I want to make sure that everything is correct before starting random vibration analysis. Thank u so much again for all your helps.

[John_Holtz · Accepted solution]

Hi @Anonymous

It looks like the option "Include rotational mass for beam elements" is affecting the results ("Setup > Model Setup > Parameters > General" tab). I ran your model with this option unchecked, and again with all lines divided into 3 divisions, and these are the mass participations in the X, Y, and Z directions:

1. 50.68%, 61.74%, 0.12% with the "include rotation for beams" checked
2. 67.71%,  83.27%, 10.19% with the "include rotation for beams" unchecked
3. 64.69%, 79.21%, 10.20% with beam elements divided by 3.

You may be able to get the X and Y participation up to 80% by including more modes (which will probably need a finer mesh by dividing the lines). I think your structure is too stiff in the Z direction compared to the total mass; you will not be able to get 80% participation in the Z direction. That should not be a problem unless you are vibrating the structure in the Z direction.

[Anonymous]

Thank u so much John for your response and I am so sorry for my late response since I was in travel and did not have access to the computer. I unchecked "include rotational mass for beam elements" and increase the number of frequency to 70 (I am not sure this number of frequency is too big or not). This time the modal effective mass percentage in X, Y and Z direction became 78%, 86% and 39% respectively. Now I am going to do random vibration analysis on my module. But I have some questions?

When I select Random vibration and go to its analysis input, under Power Spectral Density (PSD), there are three directions: X, Y and Z.

My questions are as follows:

1. Do we have to do analysis based on PSD in each direction separately? (It seems we cannot define PSD simultaneously in each of X, Y, and Z direction)

2. From where the modal effective mass percentage in Z direction is 39%, can we do random vibration analysis in Z direction or not? (Because during transportation, we usually have vibration-induced forces in all three directions)

3. In Random Vibration Analysis Input page, what are xMin, xMax, yMin and yMax, and if we want to use g^2/Hz Vs. Freq(Hz) and PSD for my case (simulation transportation-induced vibration forces on a structural component), which options should be selected under Modal Spectral Matrix Calculation: Approximation Method or Std.Numerical Integration Method, and how much "Cluster" and "Damping Ratio" should be?

Thank you so much dear John for all your helps, explanation and guidance in advance.

[John_Holtz · Accepted solution]

Hello,

1. You do not need to perform a separate analysis for each of the directions. You can click the "New" button on the Random Vibration Analysis Input dialog to define another spectrum, and choose which direction the new spectrum is for. Once you have the results, you will see that some of the frequencies respond to the spectrum in the X direction, some respond to the spectrum in the Y direction, and so on.

Note that there are some issues with this dialog. It works the first time you create the spectrum, but it does not work as well when trying to review the previous input. See the article "The Analysis Parameters for a random vibration analysis can show the wrong input in Simulation Mecha...".

2. I do not know the answer.

Correct me if I am wrong, but what I think you are really asking is this. Ideally, you want to have 80% mass participation in the direction of the PSD. Since the Z direction only has 39% mass participation, will this affect the results?

My guess is that 39% for the Z direction in this model is like 70% or 80% or 90% in a different model. Because of the constraints, some of the mass is prevented from moving in the Z direction, so it is not possible to vibrate most or all of the mass in the Z direction. In other words, the total mass participation will never approach 100% in the Z direction. I suspect that 39% for this model is acceptable, but I do not know how to prove that (other than using smaller elements and running more natural frequencies to see if the results change.) 

3. The xMin, xMax, yMin, and yMax are only for "zooming in" on the graph. (Change the values, and you will see what I mean.) These values have no effect on the analysis.

For the "Approximation" versus the "Std. Numerical Integration" methods, I suggest you look at the Help to see which one applies to your case. If you do not have any cross-mode effects, then the approximation method is a faster solution.

The Cluster value changes how the results of two frequencies of the "same value" (or "closely-spaced") are treated. If the frequency results are widely separated, then the Cluster value has no effect on the results. If there are closely spaces frequencies, what ever guidelines you are following may provide a value to distinguish "closely spaced" or "well spaced" frequencies. (If my memory is correct, 10% is a typical value (cluster=0.1).)

The damping should be the correct value for your structure. This is usually determined from physical tests on the structure.

[Anonymous]

Thank you so much dear John

Before, whenever you replied me, I would received an email, but this this I didn't receive any email. I just checked to review your previous comments and explanations and I saw that you replied my last post several days ago. I am so sorry for my late response. Thank u so much for your time and explanations. Now I am gonna work on random vibration analysis and ask you if I have any question. Just one thing. Should I create a new page and title If I have any question about the random vibration? or I can ask them in this page. Thanks

Regards

[Anonymous]

Thank you so much dear John

Before, whenever you replied me, I would received an email, but this this I didn't receive any email. I just checked to review your previous comments and explanations and I saw that you replied my last post several days ago. I am so sorry for my late response. Thank u so much for your time and explanations. Now I am gonna work on random vibration analysis and ask you if I have any question. Just one thing. Should I create a new page and title If I have any question about the random vibration? or I can ask them in this page. Thanks

[John_Holtz]

Hi @Anonymous

Yes, you should create a new topic whenever ....

• ... The topic is marked as solved. (Some people that reply to the forum posts may not read a thread if it is already marked as solved.)
• .... the subject of the post changes. If someone is looking for something, they may not read all of the posts within a thread if they see that the first post is about something different.

So please create a new thread for your random vibration questions.

[Anonymous]

Ok John. Thank you again for all your helps

Regards

[Anonymous]

Hi dear John

If you remember I already asked you some questions regarding how to intersect the lines in my Autodesk Simulation Mechanical etc. Now I have the same problem in my new model. I couldn't solve it. One of the elements of my model is not connected to other members. That's why after modal analysis, it gives me the wrong frequency value as shown in the attached image. I also attached my archive file. Could you please check my model and tell me how I can solve the issue? Thank u so much

Regards

Mojtaba

[John_Holtz · Accepted solution]

Hi Mojtaba (@Anonymous)

I think that very few of your beams are connected together. Some of the lines are not long enough to extend to meet the other beams, and many of the beams are not split. In other words, the best way to connect one beam to another is when the line segments end at the same location. It would be best if you would intersect the lines and extend them in your CAD environment, but you can also do it in Simulation Mechanical.

Once you correct the problem with the lines connecting and intersecting, you will want to divide the lines to make smaller elements to get more accurate results. In other words, you need to create a mesh.

My guess is that the lines are drawn at the centerline of the beams. In areas where one beam is sitting on another beam, you will need to add short beams to connect them together. For example, the I-beam on part 4 are somehow connected to the channel on part 2. You will need to add lines on a new part to connect those lines together, and make the new lines relatively rigid.

On a separate issue, why are you using the Nastran solver?