Youmin:
I doubt that the crash is caused by running out of memory, but I am not
sure. If insufficient RAM exists, the MAPDL solver should run fine
out-of-core. What error message is given in the output file?
To join the air and structural mesh, you need to share nodes (i.e.,
contiguous mesh) or create a contact interface(s). I recommend using a
contiguous mesh if possible.
Dan
---------------------------------------
On Wed, Nov 13, 2013 at 5:29 PM, Youmin Wang wrote:
> Hi Daniel,
>
> And attached are two simulated result files illustrating the electrical
> potential and structural displacement. As you can see there is no
> structural displacement.
>
> This is one successful computation after numerous crashing using the
> Solid226 model. I am now guess the problem of crashing could be out of
> memory, though not sure.
>
> For the no-displacement problem, i am guessing I need to create contact
> element between the air-solid interface, not sure though as well. Could you
> also give me some hints on this? Thanks.
>
> [image: Inline image 1][image: Inline image 2]
>
>
> On Wed, Nov 13, 2013 at 1:17 PM, Youmin Wang wrote:
>
>> Hi Daniel,
>>
>> I tried with Solid186 but seems it has the same problem. I have attached
>> the err file for your review.
>>
>> As an alternative, I am trying two other methods right now:
>>
>> 1. As you suggested, using workbench. I am currently in Ansys San Jose
>> training center for the 14.5 workbench training.
>> 2. Use the ROM 144 to see whether it helps.
>>
>> Thanks for your help and I will keep you updated.
>>
>> On Fri, Nov 8, 2013 at 12:50 PM, Daniel Shaw wrote:
>>
>>> Hi Youmin:
>>>
>>> If you can send me the output file from the crashed analysis, I might be
>>> able to offer some insight into the cause of the crash. R14.5 is not an
>>> unstable release for MAPDL applications. I doubt that R14.5 is the
>>> issue.
>>>
>>> Some thoughts:
>>>
>>> 1. Do not use SOLID45. It is a legacy element that is no longer
>>> supported. Use the current technology SOLID186. It will more robustly
>>> interact with SOLID226.
>>>
>>> 2. SOLID226 should work. I generally use the MFS for most electro-static
>>> structural evaluations, but the SOLID226 approach is the most recent
>>> method. It should be fine. The most critical concern for either the
>>> MFS or SOLID226 approach is excessive distortion in the air mesh. In
>>> both methods the movement of the structure distorts the air mesh. If the
>>> structure experiences large motion, the air mesh is highly distorted. You
>>> need to create an initial air mesh that is capable of being distorted into
>>> its final position. This situation is relatively unique in FE, because a
>>> coarse air mesh is often better than a fine air mesh. A coarse mesh can
>>> more easily undergo large distortion without excessively deforming any of
>>> the individual elements. Note: One of the reasons I prefer the MFS is
>>> that the structural mesh and air mesh do not share nodes. You can have
>>> fine structural mesh and a coarse air mesh. The coupled-field information
>>> is mapped across the interface. The air and structural interface share the
>>> same geometric space, but they do not share nodes.
>>>
>>> Regards.
>>>
>>> Daniel Shaw
>>> Lead Technical Services Engineer
>>> ANSYS, Inc.
>>>
>>> -----------------------------------------------------------------------
>>>
>>>
>>>
>>> On Mon, Nov 4, 2013 at 2:01 PM, Youmin Wang wrote:
>>>
>>>> Hi Friends,
>>>>
>>>> Actually, I want to state a little bit more on the meshing issue of my
>>>> current study using Solid226. The problem I have is the Ansys program
>>>> simply crashes when I try to solve. I searched online and somebody says the
>>>> 14.5 versions are not really stable. But I think it might be the problem
>>>> with the meshing. I wonder whether Daniel or anyone else has come into this
>>>> problem before.
>>>>
>>>> Thanks.
>>>>
>>>>
>>>> On Mon, Nov 4, 2013 at 11:54 AM, Youmin Wang
wrote:
>>>>
>>>>> Hi Daniel,
>>>>>
>>>>>
>>>>> Thank you for you kind help!
>>>>>
>>>>> After investigations done so far, I recognized that Trans126 element
>>>>> might not be a good choice to be used in my tilting mirror applications.
>>>>> Though the Ansys help manual indicated something as below:
>>>>>
>>>>> [image: Inline image 1]
>>>>>
>>>>> As you can see, the above figure is using Trans126 elements, though I
>>>>> think it is a simplified model. I heard that Trans126 is good for
>>>>> attraction, while difficult to perform the leaving electrodes. Beyond
that.
>>>>> I think my micromirror has more complicated geometry than the parallel
>>>>> plates, I don't know this parallel-plate simplification would be a good
>>>>> choice for it.
>>>>>
>>>>> As for now, I am considering to proceed with the Solid226 option,
>>>>> which is exactly what you have suggested. I am trying to mesh the air gap
>>>>> between the movable mirror and the fixed electrodes using Solid226
>>>>> elements, while leaving the other parts using Solid45. The electroelastic
>>>>> and structural elements are joined through nodal connectivity at the
>>>>> interface between them. I am still working on this direction right now,
>>>>> when the geometry becomes more complicated, seems it get more difficult to
>>>>> converge, I have many small parts to trim, such as the meshing and
boundary
>>>>> conditions...
>>>>>
>>>>> Another option seems to be multi-field solver, which up-to-now I have
>>>>> not acquired too much reference materials and did not dive in too deep
yet.
>>>>>
>>>>> Again, thank you very much for your help and suggestions! I am really
>>>>> grateful to you. If you could provide more insight, that would be
>>>>> great.
>>>>>
>>>>>
>>>>> On Fri, Nov 1, 2013 at 11:22 AM, Daniel Shaw wrote:
>>>>>
>>>>>> Hi Youmin:
>>>>>>
>>>>>>
>>>>>>
>>>>>> To perform an electrostatic-structural simulation using Mechanical
>>>>>> APDL
>>>>>> (aka “classic ANSYS”), you can use either the 22x coupled-field
>>>>>> elements,
>>>>>> the multi-field solver (MFS), or the electro-mechanical transducer
>>>>>> element
>>>>>> (TRANS126). You could also use the reduced order
>>>>>> electrostatic-structural
>>>>>> element (ROM144). The 22x elements and the MFS use a sequential
>>>>>> coupling
>>>>>> approach. TRANS126 and ROM144 use a matrix coupling approach.
>>>>>>
>>>>>>
>>>>>>
>>>>>> If possible, I recommend using TRANS126. It is the simplest and most
>>>>>> robust approach. With the 22x elements and the MFS, you might have
>>>>>> meshing
>>>>>> issues at pull-down. ROM144 can be complicated to implement. If
>>>>>> fringing
>>>>>> effects are significant, TRANS126 might be difficult to accurately
>>>>>> implement. In that case, you need to use one of the other methods.
>>>>>>
>>>>>>
>>>>>>
>>>>>> Regards,
>>>>>>
>>>>>> Daniel Shaw
>>>>>> ANSYS, Inc.
>>>>>>
_______________________________________________
Hosted by the MEMS and Nanotechnology Exchange, the country's leading
provider of MEMS and Nanotechnology design and fabrication services.
Visit us at http://www.mems-exchange.org
Want to advertise to this community? See http://www.memsnet.org
To unsubscribe:
http://mail.mems-exchange.org/mailman/listinfo/mems-talk