welded frame

[xLOGANx]

Good morning, guys.

I would need your opinion on a problem. I press that I'm using the wb12 of ansys. I imported it all into ansys, I set the constraints and assigned the loads. What worries me is that in welded areas, the value of tensions is low (to understand, it is blue)...and I think it is wrong given the load values I am using.

the doubt that has arisen, concerns the contact zones (connections) that are set on bonded for the whole model. Where am I wrong?

Thank you.

 

[stefano.garbin]

right-click "connections" and select "insert"->"contact tool".
once you enter the contact tool again click on it with the right mouse button and enter "status".
then, after doing the mesh, again with the right mouse button on "contact tool" and select "generate initial contact results".
What I've explained to you is to make preliminary contact control.
analyze the results well and then you can tell me okay?

 

[xLOGANx]

Thank you. I'll try immediately.

 

[xLOGANx]

Maybe the question I ask you may be stupid (or trivial) and if it were, I apologize. How do I tell him that the areas he identifies me by the method you suggested to me are welded areas?

 

[stefano.garbin]

in the contact tool controls "initial information".
you will find a tabellina where in theory all your "bonded" contacts should be "closed".
if you see "near open" or "far open" then something is wrong.

 

[xLOGANx]

errors... to understand the red ones... placed them on the minute: pins, washers and dice. in practice, only on the parts I acquire from the server we have in the studio. If, on the other hand, I delete these parts and refer to all the procedure you suggested to me, I find only 4 yellow cells: According to the legend, it is regions that are good anyway.

for bolts I think it is not important to have the 3d as long as they go to replace them with a similar bond. Am I right?

 

[xLOGANx]

Dear friends, excuse me, but I still need your help with a problem related to the " cursed" frame.
in summary:
I've run the tests hard, with ansys' wb. 13749 requires that 8 cases of analysis be defined, i.e. as many as are the combinations of x, y and z accelerations later, it is necessary to combine (to two to two) these cases, so as to obtain the deltasigma that must be compared with that provided by law.
I am proceeding very "rudimental": in places where welds will go, individual the value of stress and with a banal subtraction, obtaining a value of deltasigma to be compared.
Is there a way to combine two to two cases in ansys and get deltasigma values?
Thank you.

 

[stefano.garbin]

What you're looking for is "solution combination".
in good substance perform an analysis with 8 time passes (time=1, 2, 3.., 8)
then in the model tree with the right click do "insert"->"solution combination".
in the solution combination insert (pulsante add) the two cases to be combined with a possible weight factor.

 

[xLOGANx]

Hello stefano. Of course it works great! ! ! !
I wanted to also bring another question: I ran the 8 analyses opening 8 different tabs in the wb of ansys. There is a way, now, to connect them (I think materially) to be able to perform combinations. Do I have to raise four of the eight simulations?

Thank you.

 

[stefano.garbin]

I'm afraid you can't.
the solution combination must always share the same mesh.

 

[xLOGANx]

stefano, thank you for the answer. I hoped there was a way to connect two different "cards".
I have one last question for you. at the center of this cart (for precision, on the front) is arranged a cross welded to the longherons. I know that this traverse will have to support a mass of about 97 kg; of this mass I also have another info or that it goes to hook to two eyelets arranged on the traverse (saldati). The whole of the eyelets is a project that I know. apart from this, I do not know the shape or size of this mass.

I led the simulations with a mass point (point mass) that, by precaution, I assumed pairs to 120 kg. localization coordinates are the ones presumed by the cad model. but also asks me about geometry and location: for geometry, I have selected the cylindrical faces of the eyelets.

Is that correct? or did I miss something?
Thank you.