Mid-surface from a Solid

[Max.H.Pour]

Hi,

When a midsurface is created from a solid, what happens to the surface contacts used to exist between the solid surfaces? 

[shigeaki.k]

Hello @Max.H.Pour,

the description below applies to Nastran In-CAD (NIC) 2018.1.

In NIC 2108.1 you should find 3 types of contact: Auto, Solver and Manual. These are my findings for converting a solid part to shell using the "midsurfaces" command in NIC.

"Auto" contact

The contact made with the solid model disappears when it is converted to a shell model (see Fig.1)

"Solver" contact

The contact made with the solid model remains when it is converted to a shell model (see Fig.2). This is regardless of if the contact regions are specified or not in the "surface contact" setting dialog box. If the surfaces of the solid model was specified, these references need to be manually removed and/or modified from the "specify contact regions" box in the "surface contact" setting dialog box. The other settings such as the "Contact Type" and any other will need to be modified to account for contacts with gaps.

"Manual" contact

 The contact made with the solid model remains when it is converted to a shell model but with an exclamation mark (see Fig.3). The referenced surfaces, as well as any other settings that need to be changed to account for contact with gaps will need to be manually modified in "surface contact" setting dialog box.

                                               Fig.1

                                            Fig.2

                                             Fig.3

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Max.H.Pour]

Hi Shigeaki,

Thanks very much for your reply.

At the moment, I am trying to conduct dynamic analysis on a model (as attached).

Solidmidsurface

Converting solid bodies into shell elements by midsurface tool makes it much faster and more convenient to do various dynamic analysis. But it seems defining manual contacts between midsurface is not very easy. 

What I did was to measure the distance between surfaces and then applied 1.2 times of that measurement to max activation distance. I repeated this process for every single midsurface that I'd expect a contact there. 

 

The results are completely wrong comparing to solid analysis results which means the contacts are not defined correctly. Any thoughts? 

[Max.H.Pour]

Hi Shigeaki,

I've examined a simple model of 2 plates to compare midsurface impacts to analysis of my model. Simply, 2 plates as attached:

1. Normal Mode Analysis
2. Mesh size 4 mm , Parabolic continuous meshing 
3. Auto Bonded Contact
4. number of modes 20
5. fixed constraint 2 holes
6. Materials steel 350
7. Lowest frequency converges around 860 Hz

Converted to midsurface:

1. Normal mode analysis
2. Mesh size 4 mm, linear continuous meshing
3. Manual bonded contact between midsurfaces with max activation distance of 9.6mm, the actual model distance is 8mm
4. same materials as above
5. same modal set up
6. The same constraints
7. Lowest frequency converges around 757 Hz

It seems there is about 13% difference between the results?

[shigeaki.k]

Hello @Max.H.Pour,

could you give "offset bonded" contact a go in both models?

For contact between thin bodies meshed with parabolic solid element, current "bonded contact" is known to introduce some "stiffness" to the contact.

The alternatives are to use,

• linear elements. Mesh convergence study is highly recommend for this method, as linear elements are "stiffer" in behaviour relative to parabolic elements due to the math./theory behind it.
• offset bonded contact.
• parameter settings as per the AKN article "Model with bonded contact between thin parts behaving too stiff"

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[shigeaki.k]

Hello @Max.H.Pour,

I am following up on the post above. Could you let us know if the post was able to answer your enquiry? If so, could you click on the "Accept as solution" button for that comment. This will allow others to find the questions and answers more easily on the forum.

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Max.H.Pour]

Hi Shigeaki,

Here is the results I've got:

Solid Model:

1. Parabolic mesh 4 mm + bonded Contact = 680 Hz
2. Parabolic mesh 4 mm + Offset Bonded contact = 491 Hz
3. Linear mesh size 4 mm + bonded Contact = 928 Hz
4. Linear mesh size 2 mm + bonded Contact = 625 Hz
5. Linear mesh size 1 mm + bonded Contact = 526 Hz
6. Linear mesh 4 mm + Offset Bonded contact = 553 Hz
7. Linear mesh 2 mm + Offset Bonded contact = 518 Hz
8. Linear mesh 1 mm + Offset Bonded contact = 501 Hz

Midsurfaced Model:

1. Linear mesh 4 mm + bonded Contact = 757 Hz
2. Linear mesh 2 mm + bonded Contact = 794 Hz
3. Linear mesh 1 mm + bonded Contact = 754 Hz
4. Linear mesh 4 mm + Offset Bonded contact=794 Hz
5. Linear mesh 2 mm + Offset Bonded contact=820 Hz
6. Linear mesh 1 mm + Offset Bonded contact=807 Hz
7. Linear mesh 0.8 mm + Offset Bonded contact=795 Hz

[shigeaki.k]

Hello @Max.H.Pour,

could you split the surfaces for the contact, and apply the contact definition to these surfaces. The figure below shows an example of a split surface for one of the parts, but this needs to be done for the other part.

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[shigeaki.k]

Hello @Max.H.Pour,

I am following up on the postings. Did you have much luck with the last suggestion?

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Max.H.Pour]

Hi Shigeaki,

Results for split surfaces are:

1. Parabolic mesh 4 mm + bonded Contact = 897 Hz
2. Parabolic mesh 4 mm + Offset Bonded contact = 487 Hz
3. Linear mesh size 4 mm + bonded Contact = 922 Hz
4. Linear mesh 4 mm + Offset Bonded contact = 551 Hz

So, comparing the results with previous ones, show no serious difference. I am a bit confused here. It seems linear mesh gives more stiffness to the model so do the bonded contacts.

The question is: which combination is accurate? bonded contact and parabolic mesh? linear with bonded? linear with offset bonded? 

[shigeaki.k · Accepted solution]

Hello @Max.H.Pour,

as mentioned before, linear elements are stiffer than parabolic elements. Essentially, for thin parts, using linear solid elements may not be efficient as it will take a few layers of it through the thickness of the material to capture of the behaviour of the thin part. So I would just simply eliminate the use of linear elements in your case to simplify the matter.

I am not sure if the latest results are for shell or solids, but essentially there is an known behaviour with bonded contact and parabolic solid elements and thin parts in contact.  For solid element mesh, you can either use ENHCCONTACTRSLT=On and adjust the contact stiffness value as suggestion in Model with bonded contact between thin parts behaving too stiff while still using bonded contact.

Offset with parabolic solid elements may be another option. But you may find that the max. activation distance may affect the results. This can be minimized by having clearly defined contact areas i.e. splitting the surfaces.

If you use shell, the issue seen with the solid parabolic elements is not encountered, but you need to use offset bonded contact because of the gap in the contact. Again, in this situation, having a clearly defined contact areas help.

Regards,

Shigeaki K.