Max and Min Mesh 1

[eroque]

Hello,

Is there any way to define a Max and Min element size for the mesh. I can only aplly "Aproximate Global Size".

In Ansys i can define a min and max element size, (8 to 80 for exemple) and ansys will creat automatically a mesh with these parameters, putting smaller elements where necessary and bigger ones when possible.

Can i do this with abaqus ?

Thank u very much

 

[Dave442]

When you specify the approximate global seed size you are also given options for curvature control and min size control.

 

[eroque]

Thank you for your answer !

How can I operate with min size control ?

If i want my mesh between 8 and 80, being 80 the Aproximate Global Size, what value should i put in min size control ? (i only can choose value from 0 to 1 why ?).

Thank u very much

 

[Dave442]

This is described in the Abaqus User's Guide: "17.16.1 Defining seed density for an entire part or part instance".

First, you define an approximate global seed. Then you define a deviation factor to specify the level of local refinement in regions of high curvature. To prevent tiny elements then you can specify minimum element size as either (i) a fraction of the global seed or (ii) an absolute value.

 

[eroque]

I tried that but does not went very good.

I tried an aproximate global size of 15 and went perfect. But with this low value my mesh is too heavy and there is no need for this.

But, when i apply a global size of 50, and a min of 15 (absolute value), abaqus cant generate the mesh.

 

[Dave442]

Can you share your geometry?

 

[eroque]

Sure

So my model has 2 is a reinforced concret with 2 Parts: Concret with steel inside.

What u can see in the picture is the concret part with the steel negative inside. In assembly mode i put the 2 parts together.

The steel part i can easly mesh, the problem is in the concret part. I just need a fine mesh around the steel negative, in the concret exterior faces i can have a large elements mesh.

Thanks

 

[Dave442]

Can you specify your global seed and then specify a separate seed on the faces of the steel negative?

 

[eroque]

It´s nearly imposible. This picture is just a part of a model 10x more complex. It´s very dificult to acess the interior of the concret to seed the steel edges. And there are too many of them.

When i aplly a global seed of 15, with 0.1*15 min it´s all good. But if i put a global seed of 20, with a absolut min of 1.5 (iqual to the anterior) apears thhis image (see anex).

 

[eroque]

is there any way to mesh the al model at once ? Mesh the two parts as one.

 

[corus]

It would have been better to have a single part with the steel and concrete assigned different section/material properties, otherwise you may have a mesh mismatch between the two parts. This mismatch in mesh will cause some discontinuity in stress/temperature or whatever, and will cause problems when you try and tie all the relevant faces together.

As it stands I don't see any problem in selecting only the internal edges and assigning local seeds to them. The problem with this though, is that away from edges then the mesh will try to meet the global seed requirements and thus you'll get a coarse mesh along some parts of the steel rods. To get round this you'd need to partition along the lengths of the circular rods, say at 90 degree intervals.

 

[Dave442]

@corus: You you can assign edge seeds to entire faces so shouldn't need any additional partitioning.

 

[eroque]

Thank u for your answers !

@Corus - I already imported just 2 parts from solidworks. The steel is merged into a single part. I just have 2 parts. I already tried to seed the steel edges but the same message keeps appearing "poor boudary conditions ...", and no mesh. The only way i can mesh the steel is assigning a global seed of 15 and specifie as min 0.1*15. Any change to this wont generate mesh.

Is there any way to mesh the all model as one ? Instead of 2 separate parts ?

Thanks !

 

[corus]

@Dave442, I can't see where you assign edge seeds to a face, as that seems a contradiction in terms. However, running a test case of a solid cylinder with tet elements and applying relatively small edge seeds to the ends of the cylinder with a larger global mesh size. This did give a consistent mesh size corresponding to the edge seeds and it disregarded the global seeds, as far as I could see. The problem is I don't use tet elements generally and was just going by memory of previous times when a tet mesh wouldn't 'behave'.

@eroque, why don't you merge the two parts you have now and retain the internal edges/faces. Then assign the different materials to the separate identities and mesh it as one part, applying smaller edge seeds to the internal steel edges.

 

[Dave442]

@corus: you're right. when you specify an edge seed you can use the selection toolbar to pick faces/cells instead. I've used this before and it worked well. However, when I checked the manual, it seems that the seed is only applied to the associated edges like you suggested:

"You can select edges, faces, or cells to seed; however, Abaqus/CAE creates seeds only along edges.
When you select faces or cells to seed, Abaqus/CAE creates seeds only along the edges of the faces or
cells. In addition, you can select a set or surface to seed; as a result, Abaqus/CAE creates seeds along
the edges of the geometry contained in the set or surface."

 

[eroque]

@Corus - Thank u very much, i was needing help doing that. I have already merged the two parts in assembly mode, retaining the internal edges but ... abaqus doesn´t retain nothing and merge them completly.

I tried with a more simple exemple and works just fine. Can you please guide-me in this process ?

Thanks