Could I be right or wrong when I understand the manual section 7.43 “*DLOAD” in such manner that the axis of rotation can be any axis defined by 2 different coordinates, or should centrifugal loading always be around one of the main axis, because when I run the listed dataset where the axis of rotation is defined by (0,-5,0),(0,-5,1) I get the left picture which is obviously wrong alternative with all y-coordinates raised by 5 and axis of rotation defined by (0,0,0),(0,0,1) I get the right result shown in the right picture.

``````** Pie Cut Symmetry brick under centrifugal loading
** Unchanged Dataset will generate left picture,
**   but with all y-coordinates raise by 5 it will generate right picture
*Node
1,  1.200,   1.000,   0.000
2, -1.200,   1.000,   0.000
3, -0.800,  -1.000,   0.000
4,  0.800,  -1.000,   0.000
5,  1.200,   1.000,   2.000
6, -1.200,   1.000,   2.000
7, -0.800,  -1.000,   2.000
8,  0.800,  -1.000,   2.000
**
9,  0.000,   1.000,   0.000
10, -1.000,   0.000,   0.000
11,  0.000,  -1.000,   0.000
12,  1.000,   0.000,   0.000
13,  0.000,   1.000,   2.000
14, -1.000,   0.000,   2.000
15,  0.000,  -1.000,   2.000
16,  1.000,   0.000,   2.000
**
17,  1.200,   1.000,   1.000
18, -1.200,   1.000,   1.000
19, -0.800,  -1.000,   1.000
20,  0.800,  -1.000,   1.000
**
*Element, Type=C3D20, Elset=Solid
1,  1, 2, 3, 4, 5, 6, 7, 8, 9, 10, 11, 12, 13, 14, 15
16, 17, 18, 19, 20
**
*Nset, Nset=Center
11
*Nset, Nset=Pie_Cut_Symmetry
1,17,5,16,8,20,4,12, 2,10,3,19,7,14,6,18
**
*Material, Name=Steel
*Density
7.8E-09
*Elastic
210000, 0.3
**
*Solid section, Elset=Solid, Material=Steel
*Step
*Static
*Transform, Nset=Pie_Cut_Symmetry, Type=C
0., -5., 0., 0., -5., 1.
*Boundary
Pie_Cut_Symmetry, 2, 2
Center, 3, 3, 0
Solid, Centrif, 2741550., 0., -5., 0., 0., -5., 1.
*Node file
RF, U
*El file
S, E, ENER
*End Step
``````

Though the manual says “two points on the rotation axis are required”, further down, it says the 2nd point is the normalized direction of the axis. It looks like you’re treating it as 2 points.

@vicmw , when I saw the input deck, my first thought was, how nice, two arbitrary points in space and then the axis of rotation is defined, but obviously it’s not this way, anyway for me it’s sufficient just to know, that using the z-axis as the axis of rotation is safe, then I just can move my structure to refer to this axis

It seems that the manual is inconsistent or at least confusing. The user inputs:

1. coordinates of the center of rotation
2. direction of the rotation axis

This is also specified in PrePoMax:

And it’s the same in Abaqus:

Fixed. Sorry. I forgot updating the *Transform card,