D3PLOT 22.1

How Cut Forces are Calculated

How cut forces are calculated

Only forces in the following unblanked element types are computed: solids, (thin) shells, thick shells and beams. Other element types (e.g. springs) are ignored since Ansys LS-DYNA does not report forces in them in a way that can be read by D3PLOT. The force and moment values are integrated from the element stress & force results as follows:

Solids:
The cut face through the solid is interpolated, and its area calculated. The element stress tensor is rotated to the cut plane system and the forces are calculated from:
	Where:	Fx is in-plane X force Fy is in-plane Y force Fz is normal Z force
No local element moments are calculated within solids: they are constant stress elements. Fully integrated solids with more than one integration point. Fully integrated solids are, of course, not constant stress elements and they can support bending moments. However by default these element types only report averaged results for a single integration point at the element centre to the PTF file meaning that they are still effectively constant stress elements with no bending for the purposes of post-processing. It is possible to write data from all 8 points to the PTF file, and D3PLOT will read these results, however support within the code for this is very limited and does not currently extend to calculating local bending. This issue will be dealt with in future releases.

Thin shells:

The forces are calculated using the shell force resultants [ Fx,Fy,Fxy,Qzx,Qzy ] which yield a stress tensor in the shell local coordinate system when divided by shell thickness.

The element local stress tensor is rotated about element local Z axis to align it with the cut axis (red), giving a new system [X', Y, Z'] (green) where Z' is the same as element local Z.

The local stresses can, when multiplied by the cut area (red) give forces acting on the plane.

Sx'	* cut area	gives normal force on plane	Fx'
Tyx'	* cut area	gives transverse shear force	Fyx'
Tzx'	* cut area	gives vertical shear force	Fzx'

The cut plane is always treated as cutting the element "cleanly" in the element local Z direction, this is true even if the axis of the plane is sloping and the cut is oblique. Therefore the cut area is always (cut length * shell thickness) regardless of the obliquity of the cut..

This force vector [ Fx', Fyx', Fzx'] can then be rotated to the cutting plane system, taking into account signs.

Local element moments are also obtained by rotating the moment resultants [Mx,My,Mxy] to the cut plane axes. Warning : you should take care to distinguish between the Timoshenko convention local moments derived from stresses ( Mx, My, Mxy ) as described below, and the bending moments acting about the cut plane axes ( Mxx, Myy, Mzz ).
Mx = local bending moment per unit width due to local X direct stress. This gives rise to bending term Myy about the element local Y axis.
My = local bending moment per unit width due to local Y direct stress This gives rise to bending term Mxx about the element local X axis
Mxy = local torsion (warping) moment per unit width due to local XY shear stress This gives rise to torsion terms -Mxx and +Myy about the element local X and Y axes

The signs of the local bending moments Mxx, Myy and Mzz take into account the orientation of the cut plane with respect to the element local axes.

Shells calculate stresses in the (thin) plane of the shell, and do not develop a full 3D stress state. Therefore forces and moments in shells are reasonably accurate so long as the cut plane intersects the element "cleanly" at something close to 90 degrees as shown the the diagram below. Oblique cuts will still give reasonable results so long at the cutting angle is not too shallow. Very shallow cuts may "fall off" the edges of the element as shown on the right below, and give misleading results.

If shell force and moment resultants are not present in the database then the element neutral axis stress tensor is used instead. However

Only the mid-surface results are used , treating the element as plane stress, which means that element local bending moments are not calculated . ( Since the location of the element integration points and the degree of plasticity are both unknown it is impossible to calculate an accurate local bending moment. )

Thick shells:

Forces for thick shells are calculated by rotating stresses within the element about the element local Z axis to align with the cut plane. The cut plane is assumed to be cutting at right angles to the surface, so for best results, the cut should be close to at right angles to the surface. Local moments are obtained by rotating the moment resultants to the cut plane. Each element contributes its own individual bending moment due to the bending stresses in the element as well as the bending moment on the cut plane due to its section forces multiplied by the distance to the cut plane origin. The way forces and moments are calculated is essentially the same way as in thin shells with some differences detailed below (for more details, read the thin shell section just above this).

In thick shells, forces are calculated using the stresses at each integration point whereas for thin shells force values are extracted directly from the Ansys LS-DYNA binary output. Thicknesses are calculated using the node positions instead of being taken from the element properties. It also should be noted that force values displayed in plots are per unit length, so the cut length across each element is taken into consideration. If the element is not uniform, the length used to estimate forces is the average of the cut across the top and bottom of that element.

It should be noted that for 6 noded thick shell elements, cut section force and moment values are less accurate (compared to 8 noded thick shell elements). Also, if forces at each integration point cannot be extracted (a likely cause is a missing ztf file), the cut force will be estimated using the mid surface stress and moments calculated will be 0. The reason moments will be shown as 0 is because we would have to assume a linear stress distribution (implicitly linear elastic) which is likely to be wrong. We believe that it is better to compute no moments than a plausible but wrong one.

Beams:

Forces :

The three beam forces normally written [ Fx,Fy,Fz ] are actually a direct axial force Fx , and two transverse shear forces which should really be written Fyx and Fzx : (as in shear forces in Y and Z respectively on a plane of constant X).

This local force vector [ Fx. Fy, Fz ] is rotated into the axis system of the cut plane, taking into account signs, to give a normal force and two shear forces in the cut plane system.

Forces and moments in beams are reasonably accurate so long as the cut plane intersects the beam cleanly at roughly 90 degrees.

.Moments : These are straightforward:

The moments [ Mxx,Myy,Mzz ] are treated as a vector, and are rotated from beam local to cutting plane system and used directly.

Reporting the cut plane centroid in models containing beams

D3PLOT is able to calculate the total area cut through all elements, and hence the cut centroid (average coordinate), which enables it to report cut section results in the same "basic space" coordinate system as Ansys LS-DYNA.

For solids and shells this calculation is performed by calculating the first moment of the cut area and then dividing through by this area to obtain a centroid, but this calculation cannot include beam elements since their cut-section area is usually not known.

Therefore the following procedure is adopted when a cut plane intersects beams:

If both beam and other (solid and/or shell) elements are cut then the cut area and centroid is based on the cut area through the solids and shells only.
If only beams are cut then each is assigned a notional area of 1.0, and the cut centroid will be the average coordinate of all the cut beams. In this situation a cut area of 1.0 is always reported, regardless of the number of beams, in order to make it clear that the value is not "real".

Inconsistent beam sign conventions in Ansys LS-DYNA releases up to and including 970

Due to a bug in Ansys LS-DYNA versions up to and including LS970 exhibit the following inconsistent sign convention for beam output:

"Resultant" (typically Belytschko-Schwer) elements use one sign convention
"Integrated" (typically Hughes-Liu) elements use the opposite sign convention for 4 of the 6 output components.

The following table shows the sign conventions from releases 970 and earlier:

Component	Matching?
Fx	Same
Fy	Opposite
Fz	Opposite
Mxx	Opposite
Myy	Opposite
Mzz	Same

Sadly there is no "right" convention for beam output, as different users have different conventions. The confusion arises because of the different ways in which the beam types work: integrated beams have integration points at their centre, whereas resultant beams have (potential) hinges at their ends. The former reports force in the beam, and the latter reactions at the supports.

D3PLOT attempts to draw bending moment diagrams on the tensile side, but depending on which beam type you have used this may or may not be the case.

Beam sign conventions are consistent from Ansys LS-DYNA release 971 onwards

At some stage during the development of LS971 this problem was fixed, and results now use the "integrated" convention for all beam types. This is consistent with the reporting method for other element types in Ansys LS-DYNA, where results are the forces and moments within the element.

How D3PLOT handles the beam sign convention problem

The sign convention is crucial when computing cut forces, since the force and moment vectors are transformed into the plane of the cut, and a reversal of their sign obviously affects the answers.

Unfortunately D3PLOT can't tell from earlier results files whether an output database is from Ansys LS-DYNA 971 or later, since although the database contains a "version" field LS971 writes "970" in there! Therefore it doesn't "know" which sort of beam it is dealing with and it will ask you what beam types you have used when you first calculate cut forces through a structure. Thereafter it will apply correction factors as required . If you have mixed the two beam types in your model you will have to be extremely careful when interpreting results from a pre-970 analysis.

If you are not asked to define a system then your results file is from a version of Ansys LS-DYNA 971 onwards that is recent enough to encode up to date version information, and D3PLOT has been able to determine its format automatically.

WARNING:

Rigid elements report zero stresses, although they may still be transmitting loads. The cut forces in these elements will be calculated as zero.

Previous | Next