Centrifugal Analysis of a Propeller

[AbdulQayyum987]

I was analyzing the centrifugal forces exerted from a propeller which I have assigned it to rotate along the z-axis at 100rps. Got a fatal error when I started running the analysis. Now, do I have to put constraints for this problem?

 

[karachun]

Attach .dat and .fo6 files. You create model in Femap Student Version and therefore this file cannot be opened in regular Femap package.

 

[rb1957]

are you doing a static analysis ?

are you applying the forces as static equivalents (like m*(rw)^2) ?
radial and circumferential body forces.

another day in paradise, or is paradise one day closer ?

 

[AbdulQayyum987]

Pardon my mistake. Please find the .dat and .f06 below.


@rb1957 yes I am doing a static analysis of a propeller to determine the centrifugal force exerted by the prop while it is rotating at 100rps. The force that I applied to the model is a body force that is based on the weight of the model.

 

[rb1957]

weight body force ?
maybe you mean "mass" body forces based on the rotational accelerations ?

another day in paradise, or is paradise one day closer ?

 

[karachun]

Mesh have large aspect ratios, try to check these elements first.

Some tetrahedral elements are collapsed. Solver cannot handle with too distorted elements.
I`ve deleted some bad elements and managed to solve model.

 

[AbdulQayyum987]

@karachun, Thanks for your help. I am now able to see the deformed propeller.

If I may ask how do you manage to delete those distorted elements and missing elements means not connecting the nodes no?

 

[karachun]

- Delete elements mentioned in f06 (run Delete->Model->Elements or Delete->Model->Mesh and enter element ID from f06) and using Femap tool Tools->Check->Bad quality elements (select Aspect Ratio>=100 and Jacobian >=0,9, and set option "Make grout with distorted elements").
- Delete->Model->Nodes, select all nodes and press ok. Only nodes not connected to elements will be deleted.

 

[rb1957]

yes but that means there could (will?) be holes in the model.

I wouldn't delete elements without first interrogating them … where are they? why are they so mal shaped? how do I want the model to reconnect if I delete them?

They must have been extremely badly shaped to prevent the run from going. Normally you just get a warning ??

another day in paradise, or is paradise one day closer ?

 

[TG_eng]

Before you mesh, try running Geometry > Solid > Cleanup or Mesh > Geometry Preparation. This should help get a better mesh quality before going to solve the model.

 

[karachun]

Element deleting is urgent measure to show that problem in distorted elements, off course mesh is far away from good.

In addition - I check mesh and found that hub consist from two unconnected parts, some nodes may be merged but faces are differ.

 

[AbdulQayyum987]

@karachun..I know it is a bad mesh, then how do I improve with the mesh. Need your advise. As of the hub is concern I can use the combine tool to turn the two parts into 1 solid.

@rb1957, yes that was my initial concern. But it seems to run just fine (after deleting those distorted ones).

@TG_eng, I tried those tools before. But trust me, the geometry is more complex than that tool can handle.

 

[karachun]

@AbdulQayyum987 Attach geometry in parasolid .x_t format.

 

[rb1957]

"running fine" .NE. "giving good results"

another day in paradise, or is paradise one day closer ?

 

[AbdulQayyum987]

@karachun..Thanks alot man.

@rb1957..Please help me I'm a junior engineer. I appreciate your input in this subject matter. Appreciate it

 

[karachun]

Here is one tip. Run Mesh->Model Preparation, then build triangular plate mesh. Manually delete bad surface elements and merge nodes, you may need to create some additional elements to close holes. Then you can run Mesh->Solids from elements and create 3D mesh from 2D. Sometimes much easier to edit 2D elements than to fight with bad geometry.
Try to avoid of surfaces with corner angles near zero. You can try to rebuild geometry in CAD program before sending to Femap.

Here is my variant of mesh - I run geom. preparation, create 2D mesh and create 3D mesh without 2D mesh repair. Model run without fatal errors.

 

[AbdulQayyum987]

@karachun..I wont believe this. I have sent you the wrong file. It was actually the other one that I need your help to look into.

After creating plate elements from 2D, do I need to delete the plate elements before running analysis for solid elements?

I attach here the prop model one that I am working with..It was my bad.

 

[karachun]

Yep, or you can add solids into group and use only this group in solution if you want to remesh model later.

 

[rb1957]

make the plate elements with "plot only property" then they won't be part of the model.

another day in paradise, or is paradise one day closer ?

 

[AbdulQayyum987]

@karachun..thanks. May I have your email address if I have further questions to clarify on this subject matter.