View nodal normals visually in CAE

[zoparrat]

Is there a way to display nodal normals in CAE? So far the only way I could find to visually view any normals is from Common Plot Options to turn on normals for elements, but not the nodes themselves. And I can only view this after running a job, in postprocessing.

I can check the node normals from the .dat file, but it is a hassle.

I'm concerned about messing up the node normals when I have members connecting at acute angles, lower than 20deg.

 

[vumat721]

Aren't the nodal normals the face normals? Or am I missing something?

 

[johnhors]

"Aren't the nodal normals the face normals?"

Yes for a simple three node triangular element face.

But no for a higher order element with mid side nodes and curvature. In which case the surface normal is a function of the nodal coordinates derived using the element shape functions, and is not a constant over the element face, hence different normals at the nodes and the face centre.

I don't know of any pre/post processors which go into such detail, you are usually only required to see the element normals and in plane directions when working with anistropic material properties.

"I'm concerned about messing up the node normals"

Why? How are they messed up? Even if you could view normals at nodes, what could you do about them?

 

[zoparrat]

""I'm concerned about messing up the node normals"

Why? How are they messed up? Even if you could view normals at nodes, what could you do about them? "

I'm pretty new to Abaqus. If I understand correctly, abaqus averages node normals for to joined members, if the angle between the elements is less than 20 deg. For example, if there's a truss built with beam elements and two members are joined at a very acute angle, the node normal between these two members would be the average of the normals of the two elements. This incorrect average normal would mean that the elements have a section geometry that twists about the beam axis from one end of the element to the other.

 

[vumat721]

In CAE, you can view elements whose face corner angles (i.e. the angle between two adjacent faces) is beyond some limit (either > or < than your number). This, I presume, is the same as the "nodal normal" that you want to check? I've never used beam elements, so I don't know if this will work for you. Anyway, I believe the nodal normal is some average of the face normals near the node, regardless if you are using a linear or quadratic element.

To check this, in the Mesh Module, click the button with the picture of the mesh and the little green checkmark, or from the menu bar in the Mesh module select "Mesh... Verify...". Select the shape metrics tab in the resulting dialog.

 

[johnhors]

"This incorrect average normal would mean that the elements have a section geometry that twists about the beam axis from one end of the element to the other"

No ! Element properties are determined solely by their node topology and associated material. Other elements referencing the same nodes will not have any influence.

Just about every elementary text on FEA starts with a discussion on beam elements. You appear to be very confused, it would be worth your while studying the subject.

 

[zoparrat]

"No ! Element properties are determined solely by their node topology and associated material. Other elements referencing the same nodes will not have any influence.

Just about every elementary text on FEA starts with a discussion on beam elements. You appear to be very confused, it would be worth your while studying the subject."

I'm not making this up. Please take a look at the "cargo crane" example in "Getting started with Abaqus" documentation,
Section 6.4/Beam section orientation.
(

http://mailman.egr.msu.edu/software/abaqus/Documentation/docs/v6.7/books/gsk/default.htm)

For beams and shells Abaqus uses the same algorithm to determine the normals at nodes shared by several elements.
(

http://mailman.egr.msu.edu/software...6ch23s03alm08.html#usb-elm-ebeamcrosssection)

 

[johnhors]

"beam normals" are used to orient the beam section properties (max and min principal section axes) for any and every beam element, which for many elements in a model will usually mean the same normal direction when they share a common plane. If several beams join at a node at skew angles to each other, no longer in a common plane, then you have to specify the "beam normal" for each beam element individually as the normal direction for each element is now different to each other (no longer parrallel).


The normals for different beam elements are never averaged.

"This incorrect average normal would mean that the elements have a section geometry that twists about the beam axis from one end of the element to the other." - you are confused, this does not happen!

 

[zoparrat]

johnhors: The quoted bit about incorrect normals is directly taken from the Abaqus documentation and I referenced the location in my previous post.

 

[johnhors]

From Abaqus manual 23.3.4 Beam element cross-section orientation:-


"The orientation of a beam cross-section is defined in Abaqus in terms of a local, right-handed (t,n1,n2) axis system, where t is the tangent to the axis of the element, positive in the direction from the first to the second node of the element, and n1 and n2 are basis vectors that define the local 1- and 2-directions of the cross-section. n1 is referred to as the first beam section axis, and n2 is referred to as the normal to the beam."


"For beams in space the approximate direction of n1 must be defined directly as part of the beam section definition or by specifying an additional node off the beam axis as part of the element definition (see “Element definition,” Section 2.2.1). This additional node is included in the element's connectivity list."


which is what should be done (or as the text states "must" be defined) for beam sections (like an I or channel section). For tubes where it is not important to have a definitive beam normal direction, you can let Abaqus decide for you.