FORC_NODA: how to obtain total forces on loaded mesh faces

jmedina

Hi everyone,

I’m trying to compute the resultant forces acting on a model from applied surface pressures and compare them against the simple check “pressure × loaded area in the face normal direction.” I’m confused about the correct workflow and sign/interpretation differences between FORC_NODA and REAC_NODA. My FORC_NODA results on the loaded groups don’t match the expected magnitude and sometimes show unexpected tangential components.

If I want the resultant external force applied on a specific surface group (e.g., FACE_XPLUS), what is the recommended workflow?

Integrate pressure directly over that surface with a dedicated post-processing operator?

Sum FORC_NODA over nodes belonging to that face (and if so, should I use GROUP_NO on the face nodes, or GROUP_MA on face elements)?

Use POST_ELEM, POST_RELEVE_T with some operation instead of EXTRACTION+manual sum?

Thanks in advance for clarifying the intended use of FORC_NODA / REAC_NODA and the recommended post-processing steps to obtain face resultants consistent with p.A and with correct direction.

Julian

jeanpierreaubry

jmedina
this abstract will do the job
of course GROUP_NO='side2' has to defined before

sf=POST_RELEVE_T(
	ACTION=_F(
		INTITULE='forc_side2',
		RESULTAT=postpro,
		GROUP_NO='side2',
		NOM_CHAM='FORC_NODA',
		RESULTANTE=('DX','DY','DZ',),
		MOMENT=('DRX','DRY','DRZ',),POINT=(0,0,0,),
		OPERATION='EXTRACTION',
	),
);
IMPR_TABLE (
	TABLE=sf,FORMAT_R='1PE12.3',   

	NOM_PARA=('INTITULE','NOM_CHAM','INST','RESULT_X','RESULT_Y','RESULT_Z','MOMENT_X','MOMENT_Y','MOMENT_Z',),   

);

jmedina

Hi again, Thanks for you reply jeanpierreaubry!

I have implemented a small transient (DYNA_LINE) benchmark to verify how to correctly retrieve the external resultant force produced by a pressure load. The results still do not match the expected value using FORC_NODA, while REAC_NODA appears consistent.

Below is the corrected description of the model (in mm and N/mm²).

Model:
A clamped cantilever beam:
Cross-section: 1 mm × 1 mm
Length: 5 mm

Loaded face: 1 mm × 5 mm

Load: pressure ramped in time up to a maximum value p_\max (units: N/mm²) Boundary condition: full encastre at the opposite end

Expected resultant:

the expected resultant is: F=50×5=250 N.
With: A=5 mm² and pmax=50 N/mm

So the correct target value for verification is 250 N, purely in the direction of the outward normal.

Post-processing: FORC_NODA extracted on the loaded face. REAC_NODA extracted on the clamped face as global equilibrium check. I summed the components of both fields over time and compared them at the final loading step.

What I observe REAC_NODA summed over the fixed face correctly gives ≈ 250 N, which matches. FORC_NODA on the loaded face: does not sum to 250 N, produces extra components in directions that should be zero, even though the load is purely normal. I have attached the input files (.comm) and plots of the external forces vs reactions.

Questions for clarification

In a transient analysis, should FORC_NODA on the loaded face be expected to reproduce the instantaneous external resultant p(t)A? Or is FORC_NODA not intended as a direct pressure-integration tool?

Are the extra components in the Y/Z directions a known artifact of: distributing surface loads to nodes via element shape functions, using GROUP_NO on the face instead of GROUP_MA, mesh orientation or element type?

What is the recommended approach to obtain reliable force and moment resultants on a surface group? integrating the pressure directly over face elements , summing REAC_NODA at supports and relying on equilibrium, or another standard method?

For verification problems this small (1 mm × 1 mm × 5 mm), is there an example .comm demonstrating the “correct” way to extract the applied resultant from a pressure field in 3D?

Best regards

Julian

stage.txt

5kB

Sound_Spinning

jmedina
Nice work.
I always use node set, not an elem one, and if all good the sums in statics seem to add up OK.
I believe CA uses the stress results on elems attached to the requested area for a sum table output. Therefore, node set vs elem set, may be different. There is a whole section in the help docs about this; I'll try to find it again for you.

Update: I see in your input deck that your node sets are created off elem sets. This may mean you are using too many nodes to check on your input net load. For reactions is not a problem, as you only get 'em on constrained nodes. E.g. you can try sum of reactions using all nodes in the model and it should still give you the correct answer.

Maybe build a new node set from the UI on the loaded surf?

jmedina

Hi! Thanks for you reply Sound_Spinning!

I’m running a simulation with a very fine mesh on the loaded surface of the domain. The results improved significantly compared to the coarse mesh, but they still do not match the expected outcome for this very simple benchmark case.

The force in z direction should be 0...

Julian

Sound_Spinning

jmedina
Can you pls supply with the input mesh you are using in the run? I can take a look for you. I got your input deck (.comm), I need the mesh that goes in here: LIRE_MAILLAGE(UNITE=20)

Sound_Spinning

jmedina
Just realised you are solving this as transient dynamics?
Your thinking is for Statics, forces in Y,Z zero; have you done that 1st, a linear statics case with correct reactions?

In true transient dynamics you can get 'extra' loads. The solver models the modes of vibration depending on your time stepping; i.e. max freq defined by time inc size and number of points solved, and you can get the lateral effects on vibes. If dynamics, then it is not necessarily wrong. Try linear statics 1st.

Update:
I found the entry in docs about elem sets on reaction sums and its caveats:
Calculating the support reactions at the foot of a dam