دوستان یه توضیح دقیق از موارد زیر میخام:
1- تعریف contanctها ، برای جوش چی مناسبه، در اصطکاک چی مهمه
2- قسمت آنالیز نیوتن رالف و بقیه چه تنظیماتی باید باشه و هرکدوم کجا بکار میاد
3-وارنینگها و ارورهای زیر چیه؟
*** WARNING *** CP = 3.494 TIME= 10:02:19
Material number 7 (used by element 13281 ) should normally have at
least one MP or one TB type command associated with it. Output of
energy by material may not be available.
-------------------------------------------------------------------------
*** WARNING *** CP = 540.122 TIME= 10:07:31
Contact element 24933 (real ID 11) status changes abruptly from contact
(with target element 22226) -> no-contact.
LINE SEARCH PARAMETER = 0.2635 SCALED MAX DOF INC = 733.7
3D CONTACT ELEMENTS: 10 CONTACT POINTS HAVE TOO MUCH PENETRATION
FORCE CONVERGENCE VALUE = 0.2908E+09 CRITERION= 180.8
-----------------------------------------------------
*** WARNING *** CP = 57.050 TIME= 10:02:51
A reference force value times the tolerance is used by the
Newton-Raphson method for checking convergence. The calculated
reference FORCE CONVERGENCE VALUE = 2.849258939E-08 is less than a
threshold. This threshold defaults to 1.0-2 or is specified as MINREF
on the CNVTOL command. Check results carefully.
>>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1
---------------------------------------------------
*WARNING*: Initial penetration is included.
*** WARNING *** CP = 3.136 TIME= 10:02:18
Element shape checking is currently inactive. Issue SHPP,ON or
SHPP,WARN to reactivate, if desired.
-------------------------------------------
*** ERROR *** CP = 1209.881 TIME= 10:13:56
The value of UY at node 310 is 735802199. It is greater than the
current limit of 1000000 (which can be reset on the NCNV command).
This generally indicates rigid body motion as a result of an
unconstrained model. Verify that your model is properly constrained.
*** ERROR *** CP = 1209.881 TIME= 10:13:56
*** MESSAGE CONTINUATION ---- DIAGNOSTIC INFORMATION ***
If one or more parts of the model are held together only by contact
verify that the contact surfaces are closed. You can check contact
status in the SOLUTION module for the converged solutions using
CNCHECK.
*** ERROR *** CP = 1209.881 TIME= 10:13:56
*** MESSAGE CONTINUATION ---- DIAGNOSTIC INFORMATION ***
Rigid body motion can also occur when net section yielding has
occurred resulting in large displacements for small increments of load
or when buckling has occurred. You can plot the time history curve
for node 310 in the UY direction to check for stiffness (slope of the
curve) approaching zero.
>>> DOF LIMIT EXCEEDED. MAX VALUE= 0.7358022E+09 LIMIT= 0.000000
IT MAY BE DUE TO PREDICTOR IS ON.
PREDICTOR IS TURNED OFF FROM THIS POINT ONWARDS.
---------------------------------------------------------------------------------------
*** WARNING *** CP = 2436.907 TIME= 10:25:43
There is at least 1 small equation solver pivot term (e.g., at the UZ
degree of freedom of node 1) which may indicate a numerically unstable
model. Please check your results carefully.
EQUIL ITER 2 COMPLETED. NEW TRIANG MATRIX. MAX DOF INC= 42.72
LINE SEARCH PARAMETER = 0.2473 SCALED MAX DOF INC = 10.57
FORCE CONVERGENCE VALUE = 0.1673E+06 CRITERION= 236.6
سلام
سوال اولتون واضح نیست. خوب برای تعریف تماس دائمی مانند جوش، باید تماس Bonded تعریف کنید.
سوال دوم خیلی کلیه . قسمت های مشخصی رو بپرسید.
خطاها:
*** WARNING *** CP = 3.494 TIME= 10:02:19
Material number 7 (used by element 13281 ) should normally have at
least one MP or one TB type command associated with it. Output of
energy by material may not be available.
زیاد جدی نگیرید! معمولا برای المان های تماسی همچین پیغامی میده که تا جایی که من میدونم نیازی به اعلام این پیغام نیست. چون در تماس های متداول، ماده تعریف نمیشه.
*** WARNING *** CP = 540.122 TIME= 10:07:31
Contact element 24933 (real ID 11) status changes abruptly from contact
(with target element 22226) -> no-contact.
LINE SEARCH PARAMETER = 0.2635 SCALED MAX DOF INC = 733.7
3D CONTACT ELEMENTS: 10 CONTACT POINTS HAVE TOO MUCH PENETRATION
FORCE CONVERGENCE VALUE = 0.2908E+09 CRITERION= 180.8
یکی از تماس هایی که تعریف کردید دچار پرش ناگهانی شده. مثلا دو قطعه تماس داشته اند و ناگهان از هم جدا شده و یا درون هم نفوذ کرده اند.
-----------------------------------------------------
*** WARNING *** CP = 57.050 TIME= 10:02:51
A reference force value times the tolerance is used by the
Newton-Raphson method for checking convergence. The calculated
reference FORCE CONVERGENCE VALUE = 2.849258939E-08 is less than a
threshold. This threshold defaults to 1.0-2 or is specified as MINREF
on the CNVTOL command. Check results carefully.
>>> SOLUTION CONVERGED AFTER EQUILIBRIUM ITERATION 1
مواقعی که نیروی بسیار کمی اعمال کنید همچین پیغام ظاهر میشه و مفهومش اینه که خطای موجود از کمترین حد قابل قبول هم کمتره. بعیده مشکل اساسی ای در کار شما ایجاد کنه. البته باید مدل مورد تحلیل رو بیشناسم تا دقیق تر بتونم نظر بدم.
*** WARNING *** CP = 3.136 TIME= 10:02:18
Element shape checking is currently inactive. Issue SHPP,ON or
SHPP,WARN to reactivate, if desired.
اصلا اهمیتی نداره. چون شکل المانها در محیط Mechanical چک میشه. اصولا این پیغام نباید در تحلیل ANSYS Workbench Mechaical ظاهر بشه.
*** ERROR *** CP = 1209.881 TIME= 10:13:56
The value of UY at node 310 is 735802199. It is greater than the
current limit of 1000000 (which can be reset on the NCNV command).
This generally indicates rigid body motion as a result of an
unconstrained model. Verify that your model is properly constrained.
*** ERROR *** CP = 1209.881 TIME= 10:13:56
*** MESSAGE CONTINUATION ---- DIAGNOSTIC INFORMATION ***
If one or more parts of the model are held together only by contact
verify that the contact surfaces are closed. You can check contact
status in the SOLUTION module for the converged solutions using
CNCHECK.
*** ERROR *** CP = 1209.881 TIME= 10:13:56
*** MESSAGE CONTINUATION ---- DIAGNOSTIC INFORMATION ***
Rigid body motion can also occur when net section yielding has
occurred resulting in large displacements for small increments of load
or when buckling has occurred. You can plot the time history curve
for node 310 in the UY direction to check for stiffness (slope of the
curve) approaching zero.
>>> DOF LIMIT EXCEEDED. MAX VALUE= 0.7358022E+09 LIMIT= 0.000000
IT MAY BE DUE TO PREDICTOR IS ON.
PREDICTOR IS TURNED OFF FROM THIS POINT ONWARDS.
سیستم دچار حرکت جسم صلب شده. یعنی یکی از اجسام در راستای معینی قید نداشته و آزادانه به سمت بی نهایت رفته
موفق باشید.
