I’m having a trouble applying *DLOAD on a 1d beam edge

Please, consider the following cantilever beam example with a uniform load on the edge of 20 Nm using *DLOAD

``````*Node, NSET=Nall
1, 0, 0, 0
2, 1, 0, 0
3, 0.5, 0, 0
*Element, TYPE=B32R, ELSET=Eall
1, 1, 3, 2
*MATERIAL, NAME=MaterialSolid
*ELASTIC
210000,0.3
*BEAM SECTION, ELSET=Eall, MATERIAL=MaterialSolid, SECTION=RECT
0.1,0.3
0,-1,0
*STEP
*STATIC
*BOUNDARY
1,1,6
Eall,P3,100
*NODE FILE, OUTPUT=2d
U
*END STEP
``````

and the same beam, where *DLOAD is replaced by *CLOAD in points

``````*Node, NSET=Nall
1, 0, 0, 0
2, 1, 0, 0
3, 0.5, 0, 0
*Element, TYPE=B32R, ELSET=Eall
1, 1, 3, 2
*MATERIAL, NAME=MaterialSolid
*ELASTIC
210000,0.3
*BEAM SECTION, ELSET=Eall, MATERIAL=MaterialSolid, SECTION=RECT
0.1,0.3
0,-1,0
*STEP
*STATIC
*BOUNDARY
1,1,6
1,3,16.666666666666664
2,3,16.666666666666664
3,3,66.66666666666666
*NODE FILE, OUTPUT=2d
U
*END STEP
``````

*DLOAD gives `2.6e-02`, while *CLOAD - `2.6e-01`, which is much closer to an analytical solution

How do I apply a *DLOAD correctly? I saw the beamd.inp example, but there *DLOAD is applied on an expanded beam

Check the units. Your beam is 1x0.3x0.1 so those are probably meters, right ? But your Young’s modulus is in MPa, already suggesting inconsistent units. Then you want to apply 20 N/m (not Nm because that would be moment load). But your `*DLOAD` has a magnitude of 100. What are the units here ? And why is the same total magnitude used for `*CLOAD` ? `*CLOAD` is in Newtons but it’s definitely not the case with `*DLOAD` which is a pressure load.

DLOAD is pressure in the face, units are [F/L^2] while running load in a beam is in [F/L] units, so you need to divide your running load by the beam width to have consistency.

1 Like

@Calc_em sorry for the confusion. The beam size is in mm. I applied distibuted load of 100 N/mm simulated with *CLOAD and wanted to do the same using *DLOAD

@JuanP74 thank you for the tips - I did get the same results using *CLOAD and *DLOAD

``````*Node, NSET=Nall
1, 0, 0, 0
2, 1, 0, 0
3, 0.5, 0, 0
*Element, TYPE=B32R, ELSET=Eall
1, 1, 3, 2
*MATERIAL, NAME=MaterialSolid
*ELASTIC
210000,0.3
*BEAM SECTION, ELSET=Eall, MATERIAL=MaterialSolid, SECTION=RECT
0.1,0.3
0,-1,0
*STEP
*STATIC
*BOUNDARY
1,1,6
Eall,P3,1000
*NODE FILE, OUTPUT=2d
U
*END STEP
``````

Same with PIPE cross section (I guess because it’s expanded into a square internally)
For the CIRC cross section I found that `F / (L * Pi * D / 4)`, where `Pi * D / 4` is a quarter of curcumference, gives good appoximation - is the formula used correct?

The formula for the maximum deflection of a cantilever beam subjected to UDL is:

(8q(L^4))/(πE(D^4)) for circular cross-section

(8q(L^4))/(πE(D^4-d^4)) for pipe cross-section

(3q(L^4))/(2E(a^4)) for square cross-section

(3q(L^4))/(2Ea(h^3)) for rectangular cross-section

where q=F/L

1 Like