I have taken the IR2153 model library from the Infenion site, made the symbol of the part, and added the model file with sub extension to the path C:\Users\Product\Documents\LTspiceXVII\lib\sub
I also included it in the schematic (see beloe), but when I start the simulation, it is continuously calculating and does not finish.
It would have been thoughtful to include a link to the model, at least. I found it here and reproduced your schematic. Some models are difficult due to the way they are built, and this one is no exception (I see lots of discontinuous if() statements in there, for example) but, it seems to run. The problem is that it doesn't start immediately, it spends time during the operating point calculation. LTspice, like all SPICE engines, uses several methods for calculating it: Newton-Raphson, adaptive GMIN stepping, adaptive source stepping, and damped pseudo-transient. If all these fail then it starts from zero, as if using the uic flag. So, unless you have uic, or some other flags, set, it will try those four algorithms, and this is what happened here: it got stuck in the damped pseudo-transient mode. However, no matter which algorithm tries and fails (stalls), the usual cure is to press Esc (several times, sometimes, to skip the others, too), until the simulation starts. In your case, you may as well use .tran 10m uic, or even .tran 10m startup, they will have the same effect. Usually, those flags are not needed, or even recommended, but they have their purposes and uses. As for why it happens, that's due to the way the model is built. Somewhere, along those many lines, there are certain elements that, when the matrix solver tries to find the operating point, it fails, so it needs to skip it. Or try building the model, yourself; who know?, you may be able to make a better one. Just because a model comes from an official distributor, it doesn't mean they are all pristine.
