Menu

Discussion Forum

New Discussion
Filter

Note: This discussion is about an older version of the COMSOL Multiphysics® software. The information provided may be out of date.

Discussion Closed This discussion was created more than 6 months ago and has been closed. To start a new discussion with a link back to this one, click here.

Surface stress components on arbitrary objects

Posted Feb 12, 2014, 7:57 a.m. EST Results & Visualization, Structural Mechanics Version 4.4 5 Replies

Even Lund
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

I want to study the normal, axial and tangential stress components (full tensor) on the side surface or along a circumfering line of a conical object.

This is quite similar to a previous discussion here: www.comsol.com/community/forums/general/thread/34639/, the difference being that I want to use a boundary coordinate system instead of a cylindrical system. I am unable to use the boundary system inside the linear elastic material feature to set up this.

Could someone tell me if this is possible within Comsol and how?
5 Replies Last Post Feb 19, 2014, 11:10 a.m. EST
Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Feb 13, 2014, 4:13 a.m. EST
Hi,

A boundary system cannot be used in the material definition in a domain, since it is only well-defined on the boundary and not inside the domain.

In your case, the best solution is to create a conical coordinate system of your own using a Base Vector System under Definitions. If you call the (half) cone angle 'alpha', the axis directions would look something like

x1: cos(alpha)*cos(theta), cos(alpha)*sin(theta), -sin(alpha)
x2: -sin(theta), cos(theta), 0
x3: sin(alpha)*cos(theta), sin(alpha)*sin(theta), cos(alpha)

where theta is the angle in the X,Y-plane and Z is the cone axis.

Regards,
Henrik
Hi, A boundary system cannot be used in the material definition in a domain, since it is only well-defined on the boundary and not inside the domain. In your case, the best solution is to create a conical coordinate system of your own using a Base Vector System under Definitions. If you call the (half) cone angle 'alpha', the axis directions would look something like x1: cos(alpha)*cos(theta), cos(alpha)*sin(theta), -sin(alpha) x2: -sin(theta), cos(theta), 0 x3: sin(alpha)*cos(theta), sin(alpha)*sin(theta), cos(alpha) where theta is the angle in the X,Y-plane and Z is the cone axis. Regards, Henrik
Even Lund
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Feb 13, 2014, 12:56 p.m. EST
Thank you for the answer!

Could I use such coordinate systems only to get the tensor for one point at a time or is it possible to also do 3D surface plots and 1D stress plots along the surface? How?
Thank you for the answer! Could I use such coordinate systems only to get the tensor for one point at a time or is it possible to also do 3D surface plots and 1D stress plots along the surface? How?
Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Feb 14, 2014, 2:25 a.m. EST
Hi,

The idea is that the coordinate system is valid everywhere. This assumes that the angle theta is not entered as a parameter, but as a variable like theta = atan2(Y,X).

Regards,
Henrik
Hi, The idea is that the coordinate system is valid everywhere. This assumes that the angle theta is not entered as a parameter, but as a variable like theta = atan2(Y,X). Regards, Henrik
Even Lund
Send Private Message Flag post as spam

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Feb 19, 2014, 5:08 a.m. EST
The cone I am using have the global coordinate z-axis pointing in the direction of the top of the cone. When I use your expressions for the vectors I got a normal vector pointing slightly downwards. Everything seems correct though when changing your original expression x1, z from -sin(alpha) to sin(alpha).

Thank you!
The cone I am using have the global coordinate z-axis pointing in the direction of the top of the cone. When I use your expressions for the vectors I got a normal vector pointing slightly downwards. Everything seems correct though when changing your original expression x1, z from -sin(alpha) to sin(alpha). Thank you!
Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 1 decade ago Feb 19, 2014, 11:10 a.m. EST
Hi,

A remark: The method used here works when you have an simple boundary like a cone so that the coordinate system directions are easy to figure out. If you have a more general boundary like the title "arbitrary objects" indicates, then another method can be considered:

Add a Membrane interface to the model, and put a cladding of very thin membranes on your solid. It will not change the stiffness if the thickness is small enough. The membranes will then capture the 2D stress state on the boundary (which is correct if the surface is traction free). For the membranes, a boundary system can then be used to orient the in-plane stress components.

Regards,
Henrik
Hi, A remark: The method used here works when you have an simple boundary like a cone so that the coordinate system directions are easy to figure out. If you have a more general boundary like the title "arbitrary objects" indicates, then another method can be considered: Add a Membrane interface to the model, and put a cladding of very thin membranes on your solid. It will not change the stiffness if the thickness is small enough. The membranes will then capture the 2D stress state on the boundary (which is correct if the surface is traction free). For the membranes, a boundary system can then be used to orient the in-plane stress components. Regards, Henrik

Note that while COMSOL employees may participate in the discussion forum, COMSOL® software users who are on-subscription should submit their questions via the Support Center for a more comprehensive response from the Technical Support team.

Suggested Content