applying reaction forces of one model onto another model

[omidomidi]

i have modeled a gas turbine blade and disk separately and have done a static analysis.in a real physical model the gas turbine disk and blade are attached to each other (the bottom surface of the blade is attached to the top part of the disk).in the blade model i constrained the bottom surface of the blade in ALL DOF which after the solution creates some reaction forces.i want to put these reaction forces on my other model of the disk to perform another stress analysis on that.but the disk top surface mesh is not the same as the blade bottom mesh.the place of the nodes and their numberings are totally different but the bottom surface of the blade and the top surface of the disk are geometrically coincident.how can i apply the reaction forces of my first model onto my second model?I'm using ansys classic for my analysis.
any help is greatly appreciated.

 

[omidomidi]

any help is highly appreciated. it's urgent

 

[MrMyers]

You'll need to think about your actual situation- how are the blades attached to the disc you are modelling? Also, what are you trying to achieve? Stresses at the blade root/attachment, or far field stresses?

Is it a blisk where the blades and disc are machined from one piece?
- You'll therefore need to model the blade and disck as one part

Is the blade held by fir trees/steeples - if so, model it per real geometry! Use frictional contact between blade and disc fir trees.
To make things easier - model a slice of the disc with one blade attached - use cyclic symmetry on disc surfaces.

Are you trying to look at disc's bore hoop stress resulting from the additional blade radial loads - if so, you can calculate the radial load per blade and apply as a negative pressure distributed over the rim's surface.

Blade/disc attachments are typically precision items - your modelling technique needs to give it justice.

If you want to know stresses at the blade fixing area, using a coupling/tie constraint (that you appear to be thinking of) to transfer forces and moments across your two components will not give satisfactory results.

 

[omidomidi]

Thanks MrMyers for your help

i need to know the stresses in the disk and not in the blade or blade root. it is not possible for me to attach the blade and disk and do an analysis on it beacause number of elements increases so much and it takes so long to solve and also there are some other reasons that i can't perform such an analysis.
i have the model of the disk and the blade seprately and not attached to each other.ofcourse attaching them is not a hard job but as i said i want to analyse the disk seprate from the blade. the blade problem is solved and reaction forces of the firtree is extracted, now i need to put these reaction forces on my other seperate model of the disk (which of course is only a sector of the disk and not the complete disk) and perform a stress analysis.
the pattern of the mesh in the root firtree of the blade is quiet different from the pattern of the mesh in the coincident disk top so i can't put the reaction forces of the blade on the disk.now the quesion is here that how can i put the forces on that mesh whose node numbering is also different.
i add that also beacause of number of elements i can't do a nonlinear contact analysis.
here is the picture of the disk sector.

http://files.engineering.com/getfile.aspx?folder=f5d4f211-923f-4dbf-a828-e86c6d0e3d6b&file=disk.jpg

 

[MrMyers]

Omidomidi,

You will probably need to run a full contact solution here - the reason is because of the non-linear load sharing between each steeple 'branch'.


Imagine if the blade was modelled as rigid - the peak stress will occur on the disc's lowest fillet - but if both are modelled as elastic bodies the two parts will find an equilibrium as load is shed (by strain in the relatively thin upper disc ligament, and relatively thin lower blade ligament). The stresses at each fillet will likely be very similar.

This is particularly important where the blade elastic modulus is different to the disc modulus. (e.g. Nickel superalloy against 12Cr at mildly different temperature)

Perhaps try it out in a 2D model to see this elasticity effect.

If you don't want to model the entire blade aerofoil, and disc + contact interaction, I'd suggest you only model the blade root region (cut the blade ~20mm above the top fir tree fillet) and apply some adjusted loads to the new flat surface.

If you can't do contact at all, there are other options such as tying nodes on the load nearing surfaces to a remote point load, or similar.

Note - you can also further divide your model in symmetry/half to reduce the number of elements.
Hope this helps

 

[omidomidi]

Thanks MrMyers for your help
as i had mentioned before performing a contact analysis is not possible for my problem beacause of some reasons such as its complexity.
i think the key to my problem may be one of your last suggestions.
you said "If you can't do contact at all, there are other options such as tying nodes on the load nearing surfaces to a remote point load".
then how can i do that?
i can extract reaction forces of the blade under the blade root. but i can't apply them on the disk fitree beacuse nodes on the disk firtree are not in the place that the nodes on the blade root are.so forces are applied on a place where there is no node.
it is better to ask that "how can i apply a force on a point on a surface where there are no nodes or keypoints there."
answering this quesion will solve my problem
thanks

 

[MrMyers]

In workbench, it's probably done by using 'Remote force', this lets you tie all the nodes on one contact surface to a single node located elsewhere (you specify the x,y,z of this new point) - apply your force to that remote point to achieve distribution of said load across the surface you've tied it to.

Be careful though, as some funny/unexpected things can happen with this remote force method.

I've not used them in Ansys, but the multi-point-constraint (MPC) will let you adjust the DOF under which your constraint is active. There are probably other functions similar to MOPC to explore.

Providing you have the correct license, it may seem difficult at first, but contact isn't necessarily complex - start simple and play around (2D, frictionless) and build up from there. You'll find it'll be very useful later on.

 

[omidomidi]

thanks for your help
but i didn't finally get my answer