Hello everyone I am Ruffner. this is my first time posting a query here. I worked in a shipyard and I was tasked to know how much our keel blocks could withstand ( in terms of Tons). A keel block is a structure you put below the ship in docking so it supports the weight of the ship. I used PrePomax for structural analysis. I think made a mistake in the process but I am not sure which part of the process. So we have a model of the block. The material is mild steel and subjected to 35 tons of weight, but I used uniform pressure load of 0.8938 MPa ( that is 343232.75 N acting on 0.384 m2 of surface).
Boundary condition is Displacement/rotation U1,U2,U3 = 0 on bottom of block.
This is the result, 2.914mm displacement with deformation scale factor of 44.8. the thing I want to ask. is this accurate? I feel like the pipe should also shrink but it is not according to result. I hope you could help me.
Can you share the file ?
Make sure that all regions of this part are properly connected - if they were imported as individual parts, there can be some gaps and then without contact or other connection, load transmission won’t be correct.
This is a member under compression. Did you perform the buckling analysis?
Perhaps compound creation didn’t fully work here and some parts are still disconnected. You can run frequency analysis to check this.
You may also share files on some hosting website (like OneDrive, Dropbox or WeTransfer) and paste a link here.
Hi here is the link for the file
now that you mentioned it. I tried but Failed.
Modal analysis shows that the top ribs are disconnected from the body.
For the compound feature to work, the geometry must fit perfectly. In your case, the flanges have planar faces in contact with the cylinder, and so the geometry cannot be correctly fused.
You can try to fix the geometry - you can also combine the parts inside the CAD software that you are using. Elongate the flanges to penetrate the cylinder wall.
Or, you can use multiple tied connections between all parts using the Search contact pairs function.
Hi Matej, I followed your suggestion to elongate and penetrate the parts to ensure that the geometry fits perfectly. I acted the same uniform pressure of 0.8938 MPa in the Pipe and bracket surface and this is the result.
The whole structure shrinks by 183mm, to me this is more realistic. But how to know if this is true? That a weight of 35 Tons will actually result to this?. Btw thanks to everybody’s feedback
Use analytical calculations - simplify the geometry and check the displacement according to standard mechanics of materials formulas.
Your screenshot shows the results of linear buckling analysis. There displacements are normalized and don’t represent real values.