problem with importing geometry using igesin command

[YoonK39]

Hello, everyone
I am new to pyansys and I have a problem with importing geometry using IGESIN command.

First, I got

MAPDL Version:       22.1 (not a student version)
ansys.mapdl Version: 0.67.0

I made a simple cylinder (radius 20mm, height 20mm) with spaceclaim, just pulling up the surface to make volume, and export it to .iges file. The reason why I am using .iges is because i need to use some .step files and it can't be imported in pymapdl or mapdl just itself (is it right?).

This is my code.

mapdl.clear()
mapdl.aux15()
mapdl.igesin("D:\Folder\cylinder.igs")

When I work with a block (size all 20mm), it works. But when it goes to this cylinder model, I couldn't get a volume to analyze.

1. iges file type 186: only top and bottom areas, not volume.
   

2. iges file type 144: error occured.

 *** ERROR ***                           CP =       0.406   TIME= 15:54:29
 Poorly defined area.  Check for crossed lines.                          
 *** ERROR ***                           CP =       0.406   TIME= 15:54:29
 Cannot project lines to surface 9.  Surface could be twisted or lines   
 do not lie on the surface.                                              
 *** WARNING ***                         CP =       0.406   TIME= 15:54:29
 Unable to create 2 area(s) due to trimming problems.                    
                                                                         
 *** WARNING ***                         CP =       0.406   TIME= 15:54:29
 Entity 144 Seq 25 was not translated.  Check the original file to       
 ensure that it is ready for translation.                                
 *** WARNING ***                         CP =       0.406   TIME= 15:54:29
 Undefined line 0.                                                       
 *** ERROR 

3. iges file type 143: only areas, not volume.
   

I try to find some geometry error with spaceclaim, but it says there is no problem with the model.

I also did some job with ANSYS MAPDL.
Using type 143, it said
because keypoint merging has not been performed, automatic volume creation is suppressed

But even if i use
mapdl.ioptn('MERG','YES')
or select the merging option when importing iges in MAPDL, it failed also.

The keypoints from the model is these.

Can anyone explain why this error occurs?
I am holding this for more than a week :(

If somebody helps me, it will be a very thankful.

[mikerife]

Hi @YoonK39
Instead of exporting an iges file from SpaceClaim export instead a ANF file (Ansys Neutral Format). This is native to Mechanical APDL. Once you have the file try to INPUT it when running PyMAPDL. What happens?
Mike

[germa89]

mmhh. can you share the solid.anf file?

[YoonK39]

I'm sorry that I could not give you the original file, but I could share the cylinder file.
I have the same error when I mesh this model with mapdl.esize() command.

# Define mesh controls and generate mesh
mapdl.esize(0.5)
mapdl.vmesh('ALL')

mapdl.eplot()

The error occurs at mapdl.vmesh('ALL')

*** ERROR ***                           CP =       0.422   TIME= 15:36:28
 Unable to mesh area 3 because loop 1 has only 2 element division(s).    
 *** NOTE 

The area has 2 lines.

when I use the mapdl.smrtsize(5) command, it worked.

cylinder.zip

This is the file I am using for learning PyMapdl.

The reason I am using mapdl.esize() command is that I want a certain size of mesh, and I learnt mapdl.smrtsize() can't choose the size of mesh itself. If I am wrong, please let me know.

[mikerife]

@YoonK39 the cylinder, from the zip file, has a diameter of 0.02 so a size of 0.5 is too big. Maybe try using mapdl.esize(0.001).

[YoonK39]

It worked with the cylinder.
I would try the same solution to the original model. Thanks for your help.

[YoonK39]

Doing with the cylinder, the mesh size was the cause, but for the solid I need to use, the size wasn't the only reason.
Someone who has a same problem with me, I got the answer by using the code below.

1. Subdivide the volume. I do this because, at the first time I tried to mesh the volume, I got an error and the PyMAPDL said to subdivide the volume since the geometry is complicate.
2. Use the code below, instead just using INPUT command.

mapdl.upload("C:\solid.anf")
with mapdl.non_interactive:
    mapdl.run('/INPUT, solid, anf')
mapdl.allsel()

Although at the PyAnsys introduction page, this method is not recommended, but this was the only way that I succeed with the intended mesh size.