We are developing a chimera grids method. Wheter chimera grids method can not be applied to the case in which component speed is high? For example: The chimera grids consist of two grids: one is a large and static background grid and the other is a relatively small dynamic grid around an airfoil. The free stream Mach number is 0.3 and the airfoil is moving in the negative direction of the free stram with a Mach numer 0.5.So the flow around the airfoil is Mach number 0.8. But if the dynamic grid is not large enough, the result is obiviously not reaonable. That means chimera grids method can not be applied to the case in which component speed is high. Is it right?

No that is not right. You have some problem in your implementation. Chimera grids have been successfully applied at much higher relative velocities.

It seems a characteristic interpolation is needed. But I don't know how to do...In the above case, if the airfoil moves in the negative direction with Mach number 1.4,things get worse. The result in the moving grid seems resonable;but in the static grid, the result is wrong.

You don't need a characteristic interpolation. You do need to make sure that you have enough fringe to ensure that the interpolated boundaries don't introduce a drop in accuracy of the flux derivatives at the points adjacent to the interpolation boundary. That means that if you are using a scheme with nominal 2nd order accuracy, then you need to layers of interpolation points. This provides sufficient boundary information to allow the flux construction adjacent to the boundary to remain 2nd order accurate.

You also need to be careful that points which are moving from being hole points to field points have reasonable values. For example, if you initialize the flow field to freestream and leave the hole points set to freestream, then when one of those points becomes a field point you are introducing a sudden jump in field values unless you adjust that point's value. One approach is to average all the hole point values every time step and assign these average values to the hole points.

Thirdly, if there is a significant difference in mesh resolution in your overlap regions you can introduce a large amount of error that doesn't go away. Remember that in the overlap region you essentially have two different solutions to the equations, with the differences depending on the grid resolution. The larger the difference, the larger the error.

Are you handling the grid velocities correctly in the equation formulations? Are you correctly accounting for geometric conservation? Based on your description that the problem gets worse moving in one direction versus another, these areas are what I would look at first.

Thanks for your help. In fact,our code got very smooth resluts in overlapping region even a shock going through it when the relative speed is not high. For a store separation case, the result seems very good. But when the relative speed is high, the results are not resonable...