Error #186

It's because you created SPCD at some nodes (ex 25786) but did not create SPC there

please create both SPC and SPCD at concern nodes, values of SPCD will overwrite SPC in solver process

Dear tinh,

I have already created both SPCs and SPCDs on the same nodes. Which is why I dont understand why I am getting this error. I created a SPCADD and combined all mu SPCs. Then created a load step and defined SPCADD for the SPC and the SPCD for the LOAD. 

For the SPCD, i put a displacement value of -50 on the y-axis, do I have to put that same value for the SPC? because for the SPC, I left it at zero. 

Look forward to hearing from you

KBE

Dear tinh,

I rechecked my SPCs and SPCDs and re-did them. Now I am getting the error below.

 Element # 16752, element type QUAD4.
 ERROR - Validity limit violation: Vertex Angle =    197.47
         upper limit =    180.00

 *** ERROR # 2202 ***
 Error(s) encountered during element check
***** Element Validity Check Failed *****
 Element Quality Check Summary
 -----------------------------
 Total # of elements that failed validity check        (error) =     1
 Note: Only element with the highest violation of each check is listed below.
 Validity limit violations:

How do I find the element in fault?

Please do these steps in hypermesh

1> enter panel mask (F5)

2> select 'elems' > by id> input  16752 and press enter

3> click mask >> click reverse all

4> press F to center the elem

Dear tinh,

 

I have already created both SPCs and SPCDs on the same nodes. Which is why I dont understand why I am getting this error. I created a SPCADD and combined all mu SPCs. Then created a load step and defined SPCADD for the SPC and the SPCD for the LOAD. 

 

For the SPCD, i put a displacement value of -50 on the y-axis, do I have to put that same value for the SPC? because for the SPC, I left it at zero. 

 

Look forward to hearing from you

KBE

Please create 1 loadcollector to store SPCs, select it as 'SPC' in loadstep creation

and one other to store SPCDs, select it as 'LOAD' in loadstep creation

the value on SPC can (should) be left zero, because you may use this SPC in other loadsteps,

solver will use value in SPCD only

Thank you Tinh,

I edited the mesh manually, grouped the SPCs and SPCDs and restarted, but now I have a different error. I am working with two cylinders. Trying to encase them but they are not convergent. I changed the displacement value to something greater and im still having issues. 

Error #941 

In the contact group, DISCRET is set to S2S and TRACK is set to CONSLI. 

I await your respond

KBE

Hi,

I am not sure about the error, but if I were you, I would try several combinations, example 

DISCRET        TRACK

N2S                  SMALL

N2S                  FINITE

N2S                  CONSLI

S2S                  SMALL

S2S                  FINITE

please try and show us if any error occurred

Hi tinh,

I found the error, it was not an issue with the contact group. In the load step (NLSTAT), the NLPARM card was under NLPARM instead of under NLPARL (LGDISP). So when I changed this setting, it worked. 

Thank you for your help

Hi tinh,

 

I found the error, it was not an issue with the contact group. In the load step (NLSTAT), the NLPARM card was under NLPARM instead of under NLPARL (LGDISP). So when I changed this setting, it worked. 

 

Thank you for your help

 

 

I am just curious why OS raised an error about Contact?

I am just curious why OS raised an error about Contact?

Maybe because the contact is violated or not considered at all for a large strain problem running with a small strain formulation..?!!

I am suspecting...

 

I am just curious why OS raised an error about Contact?

 ooh, I should have mentioned that I also changed the MORIENT in the contact group to NORM and in PCONT, I activated STFEXP. It was blank before.

That might have been the reason for the contact error. Not sure though because I am new to this. 

Hi All,

i am also encountered the same error 186.

I have applied two loads in a single load collector (force and displacement). For applying displacement i have created as shown below.

<?xml version="1.0" encoding="UTF-8"?>

<?xml version="1.0" encoding="UTF-8"?>

I have defined SPC and SPCD as mentioned above. The selected nodes are same at both load collectors. Still i am facing the Error 186. Please help it out.

Hi

U have left DOF2 free, constrain it in SPC.

Thanks for your help. I have got it. 

Since in SPCD we can only able to apply displacement, please let me know how to apply the velocity and acceleration via SPCD ?

Hi

DOF for SPCD has to be referenced with SPC.

Hi @jsk459

This will be taken care as you are also applying an SPCD on the same node. 

Ya i got it.

Please help me with the below.

Since in SPCD we can only able to apply displacement, please let me know how to apply the velocity and acceleration via SPCD ?

@jsk459

You can apply velocity/acceleration in any dynamic analysis like transient or frequency response analysis.

You need to use a special load collector TLOAD#/RLOAD# to specify the load type and load curve. 

Please refer to the tutorial  OS-T: 1310 Direct Transient Dynamic Analysis of a Bracket on how to apply a dynamic load.