RECOMENDATION IN MODELLIN T-STUBS

[3JC]

Dear collages,

In this moment I'm simulating behaviour of t-stub system:

http://www.youtube.com/watch?v=8mbm2RFfrjc

I have modeled in this moment 1/2 (it's a symmetric problem) and one bolt. When I'm going to mesh I have two options (in my opinion): subdivide 1/2t-stub in three parts and constraint them with tie-option, or mesh with bottom-up option. Also I`m parametring it because I want to make a rutine to do calculations with diferents variables (such as steel grades, bolt diameters, profile and bolt dimensions, etc). Could you tell to me what is better option? Or is there a better option? I send to you in attach a screenshot.

Thank you very much,

Juan José

 

[corus]

For meshing I can't see why you can't make the whole thing structured and so need for tie options between regions. Partition it across the bolt hole and at the ends of the fillet daius.

You could do a macro for changing the bolt hole diameter but with such a simple gemoetry I'd just edit the part and properties each time.

Tata

 

[3JC]

Dear Tata:

Thank you very much for your answer. I send in attach a quickly description which regions and how I want to model (they are of articles of varios autors)

http://www.sciencedirect.com/scienc...83289b1fea1117907935cae7666016ed&searchtype=a

http://www.sciencedirect.com/scienc...5e0a95611046ac17519b5cfe47a6e96d&searchtype=a

Thank you very much,

Juan José

 

[corus]

Can't say anything about the articles as you have to subscribe in order to read them. The pdf you attached shows a very coarse mesh that would give very poor results. For instance, you have one element for the whole of the upper portion, and only one element through the thickness at the fillet radius. This will affect the stiffness of the stub and hence the way that contact works at the bolt. Partition the structure at the lines formed by the fillet radius and you should get a 'structured' shape that can be easily meshed. Be more generous with the number of elements.

Tata

 

[3JC]

Dear Tata,

Thank you very much. I've got the same opinion than you: I'll do a smaller mesh (I send to you imagen from papers because I'd like to do rules to get the mesh similar to it). In this moment I don't know what is better for my propose (I'm developing also a python script to parametrize calculations): what do you advise to me? Is better to do differents parts, or I would had to do some partitions cells with points and defineds planes?

Thank you very much,

Juan José

 

[corus]

Partition using points and planes. You can set up a macro easily and then use an input box to define specific geometry. I'd set a global mesh size so the number of elements around the bolt hole was about 40.

Tata

 

[3JC]

Dear Corus,

Thank you very much for your recommendations. I send in attach first results in meshing: in my opinion are good (I have defined three partitions in model as i send in a screenshot), but I don't like very much mesh near the bolt (I would like it could be similar to radial); so how I could do it?

Thank you very much, and in this momment I'm going to start to calculate.

Regards,

jJ

 

[3JC]

Dear collages,

After star a simulation in model send in a previous message, I have been next error:

Error in job Job-1: STANDARD_MEMORY IS CURRENTLY SET TO 256.00 MBYTES, BUT MORE MEMORY IS REQUIRED TO CONTINUE. THIS ERROR HAS BEEN ISSUED EARLY IN THE ANALYSIS. AT THIS POINT ESTIMATES OF MEMORY REQUIRED FOR THE ENTIRE ANALYSIS HAVE NOT BEEN COMPUTED.

I think that I have to increase memory destinated to Abaqus (I have a 4Gb processor). How could I do it?

Another option that I have done is to make a worse mesh. I have changed Seeds parameters, but after submit a calculation I have this message:

Too many attemps made for this increment.

How I could to solve theses two errors?

Thank you very much.

Regards,

jJ

 

[Yeray]

Dear 3jc you could edit the job, pick in job, edit, select the job, pick the tab called memory and you could increase the maximum preprocessor and analysis memory.(90%default)

regards,

Yeray

 

[corus]

The mesh still isn't very good as yuu should try and make the transition between the mesh in one partition similar to the next partition mesh size.

For the bolt hole you could partition the bolt using two orthogonal planes passing through the bolt centre. In that way you'll get a 'radial' mesh around the bolt hole. The partitions will also cut the model down the centre. Perhaps you should think of making the model symmetric along this partition so you model half a bolt hole?



Tata

 

[3JC]

Dear corus,

Thank you very much. I'm going to do partitions that you comment. When I would have results, I will tell to you. In this momment I know some problems that I had (a very high pressure, for example). But also I have a question: in this kind of problem, is it necessary to define both surfaces as slave and master? In this problem upper and lower T-stub act as slave and master, no?

Thank you very much,

jJ

 

[corus]

The two surfaces that will be in contact are defined as the slave and master surfaces.

Tata

 

[3JC]

Dear corus,

Thank you very much for your response. But, shall I have to define both surfaces as master and as slave? I use automatic detection of contact surfaces, and they are highlight in magenta or in rose when are slaves or master. So I don't know if I have to duplicate contact definitions.

Thank you very much and regards,

jJ

 

[corus]

It's not normal tp define a single surface as both master and slave, and vice versa for the other contact surface but it can be done. The problem is that when you do that then the job takes much longer to run. I'd read the manual on contact problems.

Tata