Contact Pressure of CONTA174 (ANSYS 8.0)

[Pablo]

Hi,

This is an ANSYS question. I would like to know if it is possible to get the
contact pressure at a node of an element CONTA174. I know that I can plot
with the command "PLNSOL,CONT,PRES,0,1" But what I would like to do is to
get it at a specific node attached to the contact surface. Somthing similar
to the *GET function...

Also, I would like to know what is the convention of sign (+/-) with the
CONTACT PRESSURE. In a case like the VM191 (ANSYS verification model) and
others cases (that I made my self) I found positive pressure when it is in
compression and negative when it is in tension.... In all engineering books
the conventions is that negative is associated with compression and positive
with tension, so I was wondering if people that use contacts get the same
results as I do. Thanks for your help and time.

Pablo,

[Hans-Christian Grosz]

Post by Pablo
This is an ANSYS question. I would like to know if it is possible to get the
contact pressure at a node of an element CONTA174. I know that I can plot
with the command "PLNSOL,CONT,PRES,0,1" But what I would like to do is to
get it at a specific node attached to the contact surface. Somthing similar
to the *GET function...

Did you read the section "CONTA174 Output Data" in the Element Library
of the Documentation?

Post by Pablo
Also, I would like to know what is the convention of sign (+/-) with the
CONTACT PRESSURE. In a case like the VM191 (ANSYS verification model) and
others cases (that I made my self) I found positive pressure when it is in
compression and negative when it is in tension.... In all engineering books
the conventions is that negative is associated with compression and positive
with tension, so I was wondering if people that use contacts get the same
results as I do. Thanks for your help and time.

From my understanding, pressure is always a positive force,
compressing something, like the two cylinders in vm191. Technically,
pressure can not be negative. If you pull something apart, eighter it
loses contact or there is some adhesive force necessary, which might
be expressed as a negative pressure.

HC

[Martin Liddle]

Post by Pablo
This is an ANSYS question. I would like to know if it is possible to get the
contact pressure at a node of an element CONTA174. I know that I can plot
with the command "PLNSOL,CONT,PRES,0,1" But what I would like to do is to
get it at a specific node attached to the contact surface. Somthing similar
to the *GET function...

They are available as SMISC items 1 to 4 for the 4 corner nodes;
probably most conveniently accessed by loading into the element table.

Post by Pablo
Also, I would like to know what is the convention of sign (+/-) with the
CONTACT PRESSURE. In a case like the VM191 (ANSYS verification model) and
others cases (that I made my self) I found positive pressure when it is in
compression and negative when it is in tension.... In all engineering books
the conventions is that negative is associated with compression and positive
with tension,

I think what you are seeing is correct. The ANSYS convention is that a
positive pressure acting on a face of a solid body introduces
compressive stress.

[Pablo]

Thanks for the answers. When using the SMISC with ETABLE, is there a way to
know which letter (I, J, K, L) my node is in the 4 elements it is attached
to? I would select the node, then select the elements attached to that node
followed by the ETABLE, PAR, SMISC..... to get the pressure, but to do an
average of the pressure at that specific node I need to know which letter
the node is associated to with each element.... Thanks again for the help...

Post by Pablo
Hi,
This is an ANSYS question. I would like to know if it is possible to get the
contact pressure at a node of an element CONTA174. I know that I can plot
with the command "PLNSOL,CONT,PRES,0,1" But what I would like to do is to
get it at a specific node attached to the contact surface. Somthing similar
to the *GET function...
Also, I would like to know what is the convention of sign (+/-) with the
CONTACT PRESSURE. In a case like the VM191 (ANSYS verification model) and
others cases (that I made my self) I found positive pressure when it is in
compression and negative when it is in tension.... In all engineering books
the conventions is that negative is associated with compression and positive
with tension, so I was wondering if people that use contacts get the same
results as I do. Thanks for your help and time.
Pablo,

[Martin Liddle]

Post by Pablo
Thanks for the answers. When using the SMISC with ETABLE, is there a way to
know which letter (I, J, K, L) my node is in the 4 elements it is attached
to? I would select the node, then select the elements attached to that node
followed by the ETABLE, PAR, SMISC..... to get the pressure, but to do an
average of the pressure at that specific node I need to know which letter
the node is associated to with each element....

You are getting into the wonderful world of APDL (the ANSYS macro
language).

*get,parameter,ELEM,an_element_number,NODE,a_position

(or the more elegant get function equivalent
parameter=NELEM(an_element_number,a_position)

will return the node number for a specified element at a specified
position. The position numbers correspond to the location in the
sequence I,J,K,L. Using this and a *DO loop you can identify the
position of the node in each of the selected elements.