Difficulty in meshing and solving honeycomb sandwich in ansys workbench

  • Last Post 16 October 2018
  • Topic Is Solved
vkumarsingh388@gmail.com posted this 12 October 2018

I have modelled a honeycomb sandwich according to size but when i mesh it in mechanical it takes too much time and also mesh generated is very poor and in modal analysis the result i got is wrong.

I am attaching the geometry for reference please help me by checking the geometry.

Order By: Standard | Newest | Votes
vkumarsingh388@gmail.com posted this 12 October 2018

please check if my approach for modelling is correct?

SandeepMedikonda posted this 12 October 2018

Hi Kumar,

  There are numerous posts on this forum on this topic, see if you find them useful:

  Post 1

  Post 2

  Post 3

  Also, please see if you find this post useful.

Best Practices to post on the Student Community

peteroznewman posted this 13 October 2018

Hi Kumar,

I put this image from your model here because Sandeep is not permitted to open attachments. The top skin is hidden.

You have not sliced this cleanly out of the bulk honeycomb since once cell is not closed.

The proper way to model this is with surfaces at the midplane of each solid face, not with solid bodies.

You ran a Modal analysis without holding the part, which is allowed and simulates how the part would vibrate if it was floating in space. When you do this, you have to request more than six modes, because the first six modes are the rigid body modes. You need to request seven modes to see the first natural frequency, but that might be a little off because of the missing face on one cell and the fact that you should have built it with surfaces instead of solids.

Both SpaceClaim and DesignModeler can extract midsurfaces, but they won't do the all the surfaces at once like my NX CAD system. Can you get a midsurface model from the CAD system that made that geometry?

  • Liked by
  • SandeepMedikonda
  • vkumarsingh388@gmail.com
vkumarsingh388@gmail.com posted this 13 October 2018

hey thank you for your reply and your advice.

i am new to ansys and simulation and don't use and know about midsurface, can you please tell me what is it and where to use it because i have done some simple modal analysis but never used it, so please suggest me and also how can i extract mid surface , i have model it using SOLIDWORKS.

and also while meshing i am not able to generate quad mesh properly but from where i found the problem he/she had generated the proper quad mesh with ansys APDL using SHELL181 and SOLID 186 , what are the meaning of these and how can i generate it in ansys mechanical (by using multizone mesh?).

Can you tell me is the contact given is correct between face plate and honeycomb core as i am confused about it and someone who has publish a paper on this have use contact element (contac175) and target element (target170) , what are these?

and in last As you have told me to generate more than 6 modes to get my result means if i need it find 12 modes then i have to generate atleast 12 nodes?


Thank you in advance sir. 

vkumarsingh388@gmail.com posted this 13 October 2018

sir , did i have to used share topology in design modeller to generate better mesh?

peteroznewman posted this 13 October 2018

The mesh on the solid seemed to work without share topology, but in general, it is good to use share topology when you have separate surfaces that are touching at edges. However, many CAD systems have a Sew operation that connects separate faces into one large surface body.

If Share Topology is successful, all the parts will be connected by sharing nodes at common edges and there will be no need to use contact. You can color the edges according to the Connection and the color code will tell you if the edges are properly shared. Red means a free edge, black is normal, purple is like a Tee intersection where three elements touch an edge and Yellow is like a Cross intersection where four elements touch a common edge.

Here is the SolidWorks help on Midsurface.

Once you bring surface geometry into Mechanical, the mesher will automatically create quad elements in the mesh and apply SHELL181 or 182 elements by default.

If you have a cantilever and one end of the beam is fixed, then you can find the first six natural frequencies and mode shapes by requesting six modes.  If you have no fixed support, you have to request 12 modes to see the first six natural frequencies as there are six "zero frequency" modes before any non-zero bending modes show up.

vkumarsingh388@gmail.com posted this 13 October 2018

hey peteroznewman, thank you

what is the use of Midsurface and why we have to extract midsurface?


peteroznewman posted this 13 October 2018

Say you have a 100 x 20 x 1 mm cantilever beam and you are bending it in the thin direction. There will be tension on the top and compression on the bottom. If you mesh that with solid elements, you want at least 4 elements through the thickness to transition from an element that sees tension to an element that sees compression. If the geometry is not some simple brick, but a complex thin walled solid, it can be very difficult to get a mesh that puts 4 layers of elements through the thickness. You saw that the Tet mesh you had only had 1 element through the thickness. That means a single element has to represent tension on one side and compression on the other side. It doesn't do a good job at that.

If you make a midsurface from that solid, you will have a surface that is 100 x 20 mm and you put a SHELL mesh on that. You can assign the SHELL elements the 1 mm thickness. The formulation of the SHELL element includes bending equations, so a single element is designed for bending. This is much more efficient than the solid elements. If you extract the midsurface of that complex thin walled solid, it will be easy to mesh that surface with shell elements.

  • Liked by
  • SandeepMedikonda
vkumarsingh388@gmail.com posted this 13 October 2018

thank you sir, it means it is advisable to use mid surface means i can use it everywhere and it will generate good mesh and also help in getting accurate result.

so in my model which will be more beneficial to generate mid surface in solidworks or design modeller, does it make any difference in both?

peteroznewman posted this 13 October 2018

If you generate midsurface feature in DesignModeler or SpaceClaim, when that surface shows up in Mechanical for meshing, the thickness parameter has already been filled out for you. This is very useful if you have different thickness faces.

If you generate midsurface feature in SolidWorks, you will have to define the thickness parameter in Mechanical, but you can select all and assign the thickness in one go if they all have the same thickness.

SolidWorks might create all the surfaces at once in one go. SolidWorks might trim all the surfaces to intersect properly. You have to see what works best. My NX CAD system does a great job of automatically finding all the Face Pairs and trimming them to common intersection lines.

  • Liked by
  • vkumarsingh388@gmail.com
vkumarsingh388@gmail.com posted this 13 October 2018

sir i have generated midsurface in solidworks then after importing into design modeller i have to assign thickness of surface equal to thickness of that particular solid body and then i can generate mesh in mechanical.


In design modeller did i have to select these surfaces and solid bodies to make new part as i have done earlier?


peteroznewman posted this 13 October 2018

After you make the Midsurface feature in SolidWorks, you might have to use the Knit feature to join all the separate faces into one large surface body. If you do that, when you import into DesignModeler, you won't have to do anything. There will be 1 Part, 1 Body. But if you leave the face plates or skins for the honeycomb as separate surface bodies, you will want to Form New Part of the three bodies in DM to have the mesh connect across the edges touching the face surfaces by virtue of Shared Topology. You can assign the thickness in Mechanical.

  • Liked by
  • vkumarsingh388@gmail.com
vkumarsingh388@gmail.com posted this 13 October 2018

if i have not knit the surfaces , so i have to form a part of surfaces in design modeller , so what for the solid bodies these are also imported with my surfaces i have to supress them?

vkumarsingh388@gmail.com posted this 13 October 2018

but for honeycomb core there are lots of different surfaces has generated so i have to make them 1 body so how to make it?

vkumarsingh388@gmail.com posted this 13 October 2018

i have done modal analysis on honeycomb using orthotropic material as you had mention in other posts and i got 387 modes.

and when i try it with proper modelling individual cell as you can see model above in the post i hardly get 4 nodes (when i have ask ansys to calculate 600 modes )  why this is happening, ?

i have modelled solid geometry create their mid surfaces and then made a new part in design modeller


is this approach is correct i have use orthotropic material properties for core.

I also want to do this analysis  by proper modelling cells as i have made in the model attach in the above post.

suggest me something


and thank you sir for your all advices these are very useful.

peteroznewman posted this 14 October 2018

Save As Parasolid from SolidWorks your honeycomb solid model. Put the Parasolid into a Zip file and Attach the zip file to your reply. I will show you what the midsurface looks like.

If you create midsurfaces in SolidWorks, you use Knit to join individual surfaces into one large body.

If you have midsurfaces, then you suppress the solid body.

When you do a Modal analysis, it is best to fix it to ground. Can you specify some part of the honeycomb that is fixed?

vkumarsingh388@gmail.com posted this 14 October 2018

For analysis i have used 2 approaches till yet:-

Firstly:- By using ortho material property i have generated midsurface and then make a new part in design modeller (but i am not satisfied with results).

secondly:- I have modelled the full honeycomb structure, assembled it with face plates then generated the midsurface of individual parts (core and plate)

and then make them a new part in design modeller but the model is not validated with the results we have.  


The honeycomb is not fix from anywhere as the problem specifies.

Please check our mid surfaces and help in knitting them (if possible make a video on how you are doing it)

(I am attaching both the models, please find the attachment)

Thank you.


peteroznewman posted this 14 October 2018

I opened edited assembly 1 22 midsrfc.x_t and see that it has three different thickness walls. Is this intentional?

When you sliced off a section of honeycomb, you left hanging faces like this.

It's best to delete the leftover face.

After cleaning up all the hanging faces, I have this solid model.

After using the Midsurface feature in NX, I get this set 

I could not Sew (equivalent to SW Knit) these surfaces into one body. That's okay, I will see if DM will connect the surfaces using Shared Topology.

Here is the parts in DM using Share Topology.

Here is the mesh in Mechanical. We can see that Share Topology failed because there are red lines at the Y intersection.

There is a Node Merge feature that can connect things together. The purple is correct for the Y connections.
I am a bit concerned about the black line on the one edge that should be red.

Unhiding the Top and Bottom sheets shows that the Mesh Defeaturing has connected those sheets to the honeycomb where the lines are black not red.

I defined contact elements to connect the top edges of the honeycomb to the top sheet, and the bottom edges to the bottom sheet.

Attached is zip file with the Parasolid and an ANSYS 19.1 archive.



Attached Files

  • Liked by
  • vkumarsingh388@gmail.com
vkumarsingh388@gmail.com posted this 14 October 2018

Hey peter, thank you so much for your help.

I have also made a model today by using honeycomb creator and that generated all surface body and for face plate also i have made surface body and assembled them into solidworks and in ansys i have specified thickness and also  contacts but when i am generating mesh the mesh on honeycomb core generated good quad mesh but on face plate bodies it results in very poorer mesh and also when i am trying to add sizing it fails and results in some strange mesh and workbench shows error update failed for geometry.

Mesh generated


I am attaching zip file including ansys 19.1 archive and parasloid file.

new modal analysis

please suggest me something.

and thank you for your help till now you are great and pro in this field.



peteroznewman posted this 15 October 2018

 Hey Vishal,

You have clean geometry and a good mesh. The element quality is fine. It is not necessary to get perfect squares.

Since Node Merge has connected the nodes, there is no need for any Contact elements. Delete the two bonded contacts.

You requested 30 modes. Do you know this trick to generate the mode shapes? RMB on the blank square in the Tabular data.

I recommend you characterize the honeycomb stiffness properties by fixing one end and applying a point mass at the other end and computing the modal frequencies for that case. I put a 1 kg mass on one end of the honeycomb sandwich beam and fixed the other end, then I got some sensible Modal results.

The first mode was twist.

The second mode and third mode was bending sideways.

You could compute the stiffness of each of these motions to characterize the honeycomb sandwich.


ANSYS 19.1 archive attached.


Attached Files

vkumarsingh388@gmail.com posted this 15 October 2018

Thank you so much peter, I have got the currect approach to modelling the honeycomb.

I got a doubt again as we have use surface instead of solid here (due to its benefits), and we can use it like everywhere in case of complex geometry?

As if we have to applied pressure on side face means in thickness face we will only have to use solid geometry as we cannot define pressure on thickness of surface as it doesn't allows to choose side face. so thats the limitation of its use? 

Examples if we have to do tensile or compressive test of honeycomb model we have made and the force is UDL (means pressure) so how will we can apply pressure on face plate thickness side?

Thank you in advance.

peteroznewman posted this 16 October 2018


When you put a shell mesh on a face, the mesh has the concept of a Top surface of the element a distance t/2 away from the face and a Bottom surface of the element a distance of t/2 on the other side of the face.  When frictional contact is defined to a shell mesh, you tell it if the contact is with the Bottom or the Top surface of the element.  Pressure is a bit different. It is applied to the face, and it shows with an arrow the direction the pressure will be applied. If you don't want that direction, put a negative sign on the value.