Learning Forum

[tumulpurwar]

I looked into importing a surface into SpaceClaim to use as a profile.  I created a surface and saved that as a .scdoc file then tried to select that as a Beam Profile. The first error said a profile must have a Coordinate System and a Single Colored Face.  I added a Coordinate System.  Now the error message is a Profile must have a Single Colored Face.  I don't know how to have the surface have a Single Colored Face.

Does anyone else know this?

[peteroznewman]

A simple way to create the Beam Profile from a surface you have imported is to use the Pull tool on the surface and make a solid extrusion. Then click on the Prepare tab, and use the Extract tool to convert the solid to a beam, which will create the desired Beam Profile. You can discard the beam you just created, but the Beam Profile will remain.

[tumulpurwar]

thanks...i also read this just few minutes back about the solution which you told from Spaceclaim blog, i would also like to know, that in spaceclaim, it is possible to have beam types: like truss, bar etc to choose? thanks

 

[peteroznewman]

You can convert a Beam to a Link in Mechanical, which becomes a LINK180 element. Links only carry axial force, so only the cross-sectional area A is a relevant property.

[tumulpurwar]

Thankyou for your response, in a short, can you tell or provide any weblink about various types of links like (link180, link 1, link8, Beam 188) etc...in which condition, which one can be used? and which are the popular links that are used in most of analysis queries in ansys.

well i want to know one more thing, to convert beam into truss or to convert beam in bar....same link will be use for both. that is link180?

i dont have much idea about links.

 

thankyou

[Aditya_Upadhyay]

.

Hey guys!

I am not sure about what BEAM element, 188 or 189 does Spaceclaim create when we use the extract tool. Could anyone please help? Also, Where do we change the setting for the same? Ansys Mechanical only gives the option to change from beam to truss or other models.

Would really appreciate you help!

.

[peteroznewman]

.

Aditya_Upadhyay

SpaceClaim just creates a beam element, called a line body.

Mechanical meshes the line body, just like it meshes surface bodies or solid bodies.

Click on Mesh and in the Details Window is Element Order. If you choose Linear, you get BEAM188 elements, if you choose Quadratic, you get BEAM189 elements.

.

[Aditya_Upadhyay]

.

Oh, Is that the case? Thank you for letting me know! I left the option as program controlled, so I guess I may get a mix of the two element types.

I would like to mention however that I searched the web for answers, and what I found was that, firstly, ANSYS by default models BEAM elements as BEAM188, and secondly, to specify the type of element, we need to use commands, like:

ET, 1, 188 for BEAM188,

ET, matid, 63 for SOLID63,

, etc.

There was also an answer which mentioned about midside nodes. Let me quote it. "you create a line body, and RMB on "mesh" -> "method" -> "element midside nodes" : you choose "kept" to get a "beam189", "dropped" for "beam188"."

I couldn't find this approach in Ansys Mechanical though.

.

[peteroznewman]

.

Aditya_Upadhyay

Leaving the Mesh Element Order Program Controlled allows the mesh to be appropriate to the type of solver. For example, Static Structural models will be Quadratic, but Explicit Dynamics models will be Linear. If you make it manual, and use the wrong element order for the solver, you will get an error message from the solver.

The commands you show can be used in Mechanical, but they are not necessary most of the time. The are inserted under the body in the Geometry branch of the outline in Mechanical, and use matid as the second parameter. Over time, the need for that code was reduced by exposing the functionality into the Details window. For example, code used to be required to change a BEAM188 into a LINK180 element, but now there is a Beam/Link type in the Details window for each line body.

Note that on the rare occasions when you need to insert an element type under a body, the element order on that body must match the element type. For example, if you mesh with quadratic elements, and assign an element type that is linear, that will generate an error or warning.

If you set a global setting for elements as Linear or Quadratic, you can override that setting on a specific body by RMB on Mesh and inserting a Method that can be scoped to one or more bodies. In the details for that method is an Element Order setting.

The terminology changed over time. Linear = Dropped midside nodes. Quadratic = Kept midside nodes.

.

[Claudine Adelson]

Create the surface. Extrude it using 'pull'. Change the colour of one face of the solid (click on the face and pull down menu with colour options will appear). From the Design tab, create a coordinate system. Locate it at the center of the face. Save in .scdoc. You should be able to open the file as a new Beam Profile.