Fatal Error E5000 & Warning S1126

[ttAn.autodesk]

I have been trying to figure out this error as your solved solution what shown on your forum so far but I can't. Could you figure out?

[John_Holtz]

Hi jean.par.3

It is hard to tell from an image, but my guess is that the parts of the assembly are not connected together in the analysis. How did you connect them?

1. Did you define contact?
2. Did you setup continuous meshing? If so, did you split the faces so that there are matching edges on each part? (See http://knowledge.autodesk.com/article/Does-Nastran-In-CAD-have-continuous-meshing-of-solid-elements)

What steps have you taken to try to solve the problem? For example, have you added dummy constraints and loads to all parts so that you can see what is moving and therefore not connected? Have you tried a modal analysis? (See http://knowledge.autodesk.com/article/FATAL-ERROR-E5000-SINGULARITY-DETECTED-in-Nastran-In-CAD)

If that doesn't solve the problem, then please zip the assembly and part files together (use "File > Save As > Pack and Go" if some of the part files in scattered in different locations).

[ttAn.autodesk]

Hello John,

Please see my replies in red color

your Question : Did you define contact? I defined contact as "genera'" and set tol. "0.25" (via nastran in-cad 2016) 

your Question : Did you setup continuous meshing? I set "40 mm." for element size and set "0.1" for tol. with checked on continuous meshing. (via nastran in-cad 2016)

your Question : Did you split the faces so that there are matching edges on each part? I did know how to split their faces. Which one I should do "split" or "don't split" (actually I have been following every step of autodesk's tutorial so far)

your Question : Have you added dummy constraints and loads to all parts so that you can see what is moving and therefore not connected Yes I added dummy constraints but I didn't assign load to all parts. I always checked DOF every time after I constraint or joint them and "translation & rotation" are all zero.

My previous checking : I have been checking them by assembly them part by part that, the result are fine (as my attached picture name FEA_CNPV-02.1p_case-post-1set_r1chk2, FEA_CNPV-02.1p_case-post-1set_r1chk3, FEA_CNPV-02.1p_case-post-1set_r1chk4) until I got this fatal error on "FEA_CNPV-02.1p_case-post-1set_r1chk5"

[ttAn.autodesk]

Hello John,

Here is my pack & go file for you to figure out.

NOTE#1 : My pack & go file (jean.par.3.zip) have been created via Inventor 2017 & Nastran In-cad 2017 but this fatal error caused on previous version of Inventor & Nastran In-cad

NOTE#2 : I don't understand why they fine if I analysis them via "Stress Analysis" of Inventor but I couldn't analysis them via Nastran In-cad.

[John_Holtz]

Hello,

I see that you have two analyses set up in the model:

1. One in which the Surface Contact is "Auto". This analysis fails with the E5000 error. It is not too easy to locate the node 14881 (the grid number mentioned in the error), so duplicating the analysis and running it as a modal analysis is the easier way of finding what part is not statically stable. The modal analysis shows that the two M16 nuts are not connected to the model. This would be a problem when doing a static analysis.
2. A second analysis in which the Surface Contact is defined manually for each pair of surfaces in contact. This analysis runs successfully.

I think the reason the first analysis fails is because there is an interference between the nut and the bolt, so the automatic contact doesn't detect that they should be bonded. When you define the contact manually in the second analysis, it is able to create the contact in spite of the interference. (The bolts and nuts do not have threads; that is just an image in Inventor. So maybe the "bore" through the nut uses the ID of the thread and the "cylinder" of the bolt uses the OK of the thread, and this results in an interference fit between them?)

Since you have defined that all of the parts are bonded, you have several options:

1. Suppress the bolts, nuts, and rods. They are not providing anything useful to the analysis. Since the parts are bonded, they will not come apart.
2. If you need a more refined analysis, then you need to define separation contact between the parts of the bracket. Be aware that this analysis then becomes an iterative solution to determine which nodes are in contact and which ones are not, so the run time will be longer (maybe much longer depending on the analysis).
   1. Then the preferred method of doing the bolts, nuts, and rods (to hold the components together) is to add connectors (right-click on the Connectors branch of the browser) to simulate the bolts and nuts.
   2. If you need to include the "real" bolts and nuts, you can include them and define the proper contact between the parts.

[ttAn.autodesk]

Hello John,

• Could you instruct me how to detect the problem as you informed regarding "Modal Analysis"? Because I will analyze further error on my next project via Modal Analysis. My attached zip file name "Modal Analysis" are shown nothing related nut & bolt M16.
  
  
• I have tried to analyzed on actual nut & bolt (I created my own nut without thread for eliminate interference) with "separation" on surface contact that, I got the same fatal error.
• My attached jpeg file name "FEA_CNPV-02.1p_case-post-1set_r1chk6" is the result which I analyze on actual nut & bolt (I created my own nut without thread for eliminate interference) with "bonded" on surface contact. Could I refer this result for the proper Stress Analysis one?

[John_Holtz]

Hi,

If a model has a part that is not statically stable, and therefore gives an error E5000 during a linear static stress analysis, doing a modal analysis will show where the problem occurs as follows:

1. The lowest frequency will be very close to 0.
2. The part that is not connected to the model will move; the rest of the model will have a displacement of 0.

The images that you attached in "Model Analysis.zip" look to be for a model that does not give error E5000. Is that correct? All of the mode shapes shown in the images look to be valid vibration of the model.

[ttAn.autodesk · Accepted solution]

Hello John,

1. Thank you for your instruction regarding "How to analyze result of Modal Analysis".
2. Regarding an image of my result of Modal Analysis. That is correct it didn't gave error E5000. After that I assembly them to be a completed set as followed detail

Assembly

• Nut & Bolt : To prevent Interference issue , I created nut without "threads" (for FEA). I didn't apply nut from content center.
• Constraint & Joint : To prevent Degree of Freedom issue , I constrained and joint every part more than 2 points (translation = 0, rotation = 0).

FEA

• Surface Contacts : To prevent Fatal Error E5000 issue , I set them in Auto ; Bonded for contact type ; specify contact regions on Body (neither face nor edge) of entire parts and fasteners.
• Mesh Model : To prevent Mesh Failed issue and Fatal Error S1110 , I defined their mesh via Mesh Table with value 1.25 to 40 mm. for element size and 0.01 to 0.1 mm. for tolerance on necessary parts and fasteners; 150 to 200 mm.for element size and 1 mm. for tolerance on unnecessary parts. Moreover I set virtual memory as follow as Window recommended.

The result shown "SUCCESSFUL"

NOTE : I analyze them via Inventor v.2017 & Nastran In-CAD v.2017 and this Fatal Error occurred on previous version of Inventor & Nastran In-CAD. On previous version of Nastran In-CAD sometime the result after solved it not shown "Solid Von Mises in result data"

Thank you

John