mesh control 3

[ChessFalconer]

Hi
I´m making a job with ANSYS and I use smrtsize function to mesh my solid. I want to study the propieties in a very particular place of the solid (but I need to built the whole solid which is quite complicated, and substructuring is not posible) then I want a fine mesh in a specific zone and a coarse one in the rest. If i use the smrtsize the function makes a mesh which is more fine than necesary but not good enough in the place where I want. I cant use a low number for smrtsize because the problems turn a huge one for any PC.
Is there any COMMAND (I don´t want GUI procedures) to solve this problem?.
I will try to break my solid in two ones and them glue the surfaces, then i can make a coarse smrtsize in the main part and a fine in the problematic zone. But at this point I think that this can introduce other type of problems (ie warning about tetraedrics angles)that´s why I want your opinion. Do you think that solution could be a good one? Have you got a better idea? Thank you very much

 

[doatis]

ChessFalconer,

The more you use ANSYS, the more you realize smrtsize isn't necessarily the best solution. Whenever I want to control my mesh density, I use mesh200's, set to be a 6-node triangle if I'm meshing with solid quadratic tets. You can then go through and 'seed' mesh all your areas of concern with a small element size (esize... followed by an amesh,p).

Once you understand how the ANSYS mesher works, it will make more sense. First, it goes through and creates all the line divisions, then meshes each area, and finally grows the mesh inwards. If you have already defined line sizing (lesize) or meshed an area, it will simply use that instead of trying to figure it out yourself.

The old way to do this was to mesh your "problem" areas first with shell elements, then delete those elements before the solution (don't want to add a hard candy-shell to your model). The mesh200's do the exact same thing, except they are not solved. The only options you define are the shape of the mesh200 (i.e. the element face for the element you ultimately want to use).

Hope this helps,
Doug

 

[ChessFalconer]

looks like I have to study more. I will try you sugestion, I have to take a look to documentation about commands you sugest. thanks!!. This is all... by the moment

Jose (studing new commands)

 

[meshparts]

I submit to what doatis wrote. Manual meshing control is better then smart size.

To the problem with smart sizing: there are options how control how mesh expands, see the EXPND option on SMRTSIZE command.

Regards,
Alex

 

[doatis]

Just to follow up on Alex's suggestion:

You also have those same expansion controls outside of the smrtsizer. Look up the documentation for mopt. The two options I use are expnd (how fast an area mesh grows from the line sizing to the global sizing) and tetexpnd (how fast a volume mesh grows from the area sizing to the global sizing).

Enjoy,
Doug

 

[ChessFalconer]

Thanks everybody for the sugestions I´m really learning a lot.
Ok my problem is that a have a solid with a number of holes, this number changes because I´m making a *.lgw file to solve many problems (dependns of the value given by a *SET command). I know the place where the holes are going to be made but I don´t now more (I´m just looking for the best combinations of holes in a solid for some solicitations). I just want a fine mesh (as fine as posible) in the place where the holes are and a coarse one in the rest (that´s why I know that the mechanical problem is in the holes). But I need to put all this in my *.lgw file. will be fantastic if I could said to ANSYS: "Please mesh with a fine mesh the geometry inside the area defined by this four points and with a coarse mesh the area outside".

The mesh200 idea of doit as I understand is to make a first mesh in the problematic zone and them re-mesh all (because ANSYS will use the meshed area as was meshed). The problem is that the place where i want to mes (the exact place) depends on the number of holes. I have to see more that command, look powerful and I need more time to study it.

If I want to use "The old way" to do this sugested by doatis (to mesh your "problem" areas first with shell elements, then delete those elements before the solution). I will have to use a *DO *ENDDO to fit this with a *.lgw file which can be used with diferent numbers of holes. Looks that could be a solution, I find more easy my first idea (see my firt post) but probably "The old way" makes a better job. I have to try it, I know the number of the last line and area created before the holes are made then I could try a *DO *ENDDO. I will tell you my experiences

The use of EXPND in SMRTSIZE function look that is not correct in this problem because smrtsize has no way to understand where i want a fine mesh, is usefull to control how the mesh grows from a line to a volumen but no in my problem (I need this control in a particular place not the whole solid). Similar conclusion can be made for MOPT suggestion.

I supose the good way is to use *DO *ENDDO with manual mesh of the lines involved in the holes and then go to areas and the rest. But look dificult to find the lines number with a *DO *ENDDO the same problem of "the old way" (i need my *.lgw for any number of holes)

I really say you THANK YOU because I´m learning a lot, and with your suggestion I have a idea of where the solution could be, please give me your sugestions, ideas are really apreciated. In the following day I have more time to work on my ansys job (last days I have no much time) them I could give you my impresions and...solutions??

Thanks!
Jose

 

[DonTonino]

Have you tried creating one or more components out of the areas (for example) that belongs to the holes you are making? Knowing the location of the holes, you can select the areas by location (switching to a polar coordinate system centered on the hole center and selecting every area between r-x and r+x, being r the hole radius and x a small value, for example), making a component out of them and then issuing a mesh command
to apply the fine mesh. You can also do away with the component making of course, I just usually find components quite useful while working in batch mode as once you have it defined you can issue any number of commands referring to the components, instead of having to reselect every time whatever you want to work on.

 

[meshparts]

Another possibility to what DonTonino proposed, is to select line belonging to the hole by the length.

Usually o circle in Ansys has 2 or 4 equal lines. If you know the radius of the holes, you can select them by

pi=acos(-1)
lsel,s,length,,(2*pi*rad)/2
lsel,a,length,,(2*pi*rad)/4

 

[doatis]

If you know your 4 points that define the mesh-refinement zone, why not create a box and perform a boolean overlap. You'll have to be careful with your volume numbers, but they you will have a distinct volume which you can specify a smaller mesh size (either esize or smrtsize). You can then increase the sizing and mesh the rest.

Hope this helps,
Doug

 

[ChessFalconer]

the problem is solved with the vovlap command sugested by doatis (is similar than the idea i had in my fist post as you can read in the upper), this is the first solution and probably not the best one. I simply do what doatis sugested I used glue command in combination with vovlap.
1) create an new volumen to define the area where the holes are going to be done
2) use vovlap command with the new area and the area where the holes are going to be done
3) delete the auxiliar area
4) glue the new areas
5) mesh each area with diferent smrtsize value

Now I want to solve the problem with the indications given by dontonino (areas) and mihaiupb (lines) looks more dificult but also better result are expected. I will gime you my result in next days.

Thank you very much I continue working and learning!! Of course I apreciate more sugestions
Thanks dontonino mihaiupb and doatis

Jose