turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Simcenter 3D Forum
- Surface to surface contact

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-21-2015 11:51 PM

Hello guys,

I am attempting to simulate a peristaltic pump. The model consists of a bar with rounded ends and a tube that goes around a diameter equivalent to the length of the bar. The bar is supposed to be compressing the tube at the contact region but since it has been modeled using actual dimensions, the bar and the tube are overimposed. A surface-to-surface contact has been defined between the rounded end of the bar and the inner wall of the tube. Both tube ends are fixed as well as the bent region (to simulate contact against a wall). The center of the bar is also fixed for the static analysis before turning the pump.

Before attempting any motion or dynamic analysis, I wish to try a static analysis to determine the force, stresses and deformation resulting from the contact only. Afterwards, I'll try to complete a motion simulation (something like this: https://youtu.be/DGBfLxwyS6Y). When I solve with the Sol101 solver, I get some unexpected results. It looks weird like the bar penetrating the tube. I am pretty sure that the issue might be related to the contact definition or some related parameter. I have included the simulation files.

Thank you for your assistance

Labels:

3 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

10-22-2015 07:20 AM

Hello!,

I am sorry to tell you but linear static analysis (SOL101) is useless in this case, you have a nonlinear problem because large displacement effect are present in the problem, you need to use ADVANCED NONLINEAR ANALYSIS (SOL601). This is an interference-fit problem, then you need to use a negative minimum search distance to account for the interference and get the solver to move any component to its final position.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

11-12-2015 09:26 PM

Thank you, Blas

I appreciate your response. I tried the Sol 601 but it did not run. I suspected something was wrong with the model so I decided to remake the model. Afterwards, at least it started running but now I'm getting a negative jacobian error. I've tried remeshing with smaller element sizes to no avail. I know I am missing something simple. It even tells me which is the element but I do not know how to identify and correct that element.

It has come to my mind to split the bodies to refine the mesh in particular regions but I would like to make sure which elements are causing the error before trying something.

Any thoughts? I included the model files.

Thank you

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

11-16-2015 03:11 PM

Hello!,

First at all you need to prepare the geometry to mesh effciently with HEX elements, avoid to have 3-D solid TETRA or 3-D solid triangular prismatic elements, the best one is the CHEXA elements. If you prepare the geometry (either is the master or idealized model) like this way slicing the solid tube & dividing the surface of the block using a 2D SEED mesh to control the quality of the 3-D solid mesh then you will have a correct mesh to work with the analysis options.

The 2-D Seed mesh using command "2D Mapped Mesh" is the following (make sure to desactivate the option "**export mesh to solver**"):

And then the 3-D solid Hexaedral mesh is really easy to create using command "3D Swept Mesh", here a CHEXA 20-node elements were create to account for effective contact between parts (later in NXSTRAT command of NX NASTRAN ADVANCED NONLINEAR (SOL601,106) make sure to convert CHEXA 20-nodes to 27-nodes (with extra midside nodes) using ELCV=-1 under NXSTRAT > TRANSLATION):

Also, in the FEM environment you need to define the material properties of the components: please note if the TUBE is a rubber-like material the you need to enter the **nonlinear HYPERELASTIC material properties** using, for instance, either the MOONEY-RIVLIN, ODGEN or ARRUDA-BOYCE constants; this is a critical steep in the simulation because is difficult to have the correct information available.

Later in the SIM environment you need to define important data using the **Modeling Objects Manager** like Time Step, SOL601 NXSTRAT Strategy parameters, Surface-to-Surface Contact parameters for the Advanced Nonlinear Pair, the Structural Output Request, etc..

For the Contact setup, here you have two options:

- One is the current option: you have defined the two bodies withing the initial position, then the SOL610 solver will "resolve" the penetration (INIPENE=0) and will move each body to its equilibrium position depeending the material stiffness. In this case remember to set a
**negative MIN SEARCH DISTANCE**in the contact pair set properties (BCTSET card) to let the solver to "resolve" the interference fit, the value to enter here should be the current geometric interference, but in negative form, OK?. - Two: alternatively you can separate both bodies to avoid any phisical interference and prescribe an
**enforced displacement to one end of the block**to reach the current "penetrating" position, then the solution of both contact stress & resultant displacements at the end will be more or less the same.

The solution is not easy, the convergence in this type of nonlinear contact problems is critical. In the NXSTRAT card select Automatic Time Stepping (**ATS**) and select the 3D-Iterative solver, because the model has high-order CHEXA 27-nodes elements it should speed the solution.

To learn more about Advanced Nonlinear I suggest to run the TUTORIAL EXAMPLE under **NX 10 HELP > CAE > Tutorials: Advanced Simulation**, this way you can make us specific questions, not how to run the full model, OK?.

Best regards,

Blas.

Blas Molero Hidalgo, Ingeniero Industrial, Director

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

IBERISA • 48004 BILBAO (SPAIN)

WEB: http://www.iberisa.com

Blog Femap-NX Nastran: http://iberisa.wordpress.com/

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc