[转帖]接触单元常问的问题及解答

simon21 · 发表于 2005-8-18 17:15

马上注册，结交更多好友，享用更多功能，让你轻松玩转社区。

您需要登录才可以下载或查看，没有账号？我要加入

x

这是从XANSYS上转下来的, 挺好, 值得一读: %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% F. A. Qs on CONTACT - ANALYSIS %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% Terminology: STS - Surface to Surface Contact NTS - Nodes to Surface Contact NTN - Node to Node Contact FKN or Kn - Normal Contact Stiffness E - Youngs Modulus ICONT - Initial Contact value PMIN & PMAX - Minimum and Maximum initial Penetration range PINB - Pinball region Radius FTOLN - Penetration tolerance Mu - Friction Coefficient %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 1. On what factor can a contact analysis be judged as "OKAY"? ======================================= Answer: Penetration. In physical reality, penetration between 2 contacting bodies never occurs. This is a mathematical creation so as to activate a contact stiffness between two bodies. Keeping penetration to a minimum is a best way to simulate a contact analysis. For acheiving this, the contact Stiffness may be specified as high as possible as long as a converged FE solution is possible. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 2. What affects the accuracy and convergence of a contact analysis? ======================================= (FKN) Stiffness used for the Contact is a major factor affecting Convergence of Contact problems. Using Higher values of Stiffness may diverge the solution. Its advised to start with a small enough value and get a converged solution. Re-solve with increased value of stiffness so long as the problem stops converging. Trial-and-Error + Experience will help you predict the Contact Stiffness needed to solve a Contact Analysis. Another recommended practise is to run the analysis with an initial small contact stiffness and then slowly increase the stiffness over a series of load steps. This will ramp the contact stiffness value from the initially considered Stiffness, thus improving convergence behavior. The results for the last loadstep would have been analysed with more stiffness and hence would be more accurate than previous results. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 3. What is Hertz Stiffness? How is it calculated? ======================================= Hertz Stiffness provides an approximate value for the Penalty Stiffness value. Kh = l*E where, Kh --> Hertz Stiffness l --> Size/edge length of the element at the contact surface E --> Youngs Mod of Contact Surface For 2D models, the thickness of element is considered for l %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 4. Simulating contacts between 2 Rubber material bodies. How can I evaluate E for the rubber so that I can roughly estimate the contact Stiffness? ======================================= Consider E for the rubber material portion as: E = 6(a+b) where a and b are the first two Mooney-Rivlin contants %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 5. While using NTN contact elements between two (3D) surfaces, is there any recommended practise for meshing at those two surfaces? ======================================= Meshing between the two sides were varying along X. Surface 1 - - - - - - - - --- --- --- --- --- --- --- Y $ $ $ $ $ $ $ $ $ $ $ $ $ $ $ | - - - - - - - - --- --- --- --- --- --- --- |___ X finer coarser Surface 2 $ sign indicates the Node-To-Node Contact Element between the Nodes of Surface 1 and 2 respectively. If you observe the mesh variation along X direction, it has varied from Finer to coarser. In such situations, use of a uniform Kn value for all the N-T-N contact elements could lead to un-even contact pressures. It is advisable to specify different values of Kn. If this step was not taken care of, then the finely meshed portion will experience more stiffness compared to the coarsely meshed portion. To avoid these issues, its recommended practise to use the same edge length between the two surfaces 1 & 2.

simon21 · 发表于 2005-8-18 17:16

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 6. What are the guidelines to estimate FKN for a contact Analysis. ======================================= For bulky contact, where the two are solid bodies FKN = 0.1 to 10 ---> Factor of E For contact between two slender bodies ( thin / bending dominated structures) FKN = 0.01 to 1 ---> Factor of E Its always advised to start with a lower value of FKN and proceed later with higher values. The default setting in Ansys is 1, irrespective of what kind of bodies are participating are getting in Contact. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 7. When two different material (say Steel and Aluminum) are in Contact, which material's E should be considered for evaluating FKN ======================================= E of the softer material be always considered for estimating FKN. In this case prefer E of Aluminium. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 8. How to specify Sticking and Sliding conditions for Contact between two bodies. ======================================= 'Mu' - Friction coefficient and TAUMAX are the two inputs user needs to specify. If Ft >= Mu*Fn where Fn --> Normal Force & Ft --> Tangential Force, the bodies slide relative to each opther and the two contacting bodies experince a Shear force of TAUMAX. Sticking happens when Ft < Mu*Fn %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 9. How to estimate TAUMAX? ======================================= TAUMAX = (Von Mises Yield Stress/1.732) This is an empirical formula %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 10. I have Higher order elements (with mid-side nodes) on the two contacting surfaces & I want to analyse the problem using NTN Contact. Can I create NTN Contact between the mid-side Nodes? ======================================= Due to the uneven nature of the kinematically consistent reaction forces at the nodes of midside-noded elements, NTN contact should NOT be applied to mid-side nodes. In effect, usage of NTN implies that only lower order elements be used for underlying mesh of contacting parts.

simon21 · 发表于 2005-8-18 17:16

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 11. While editing the real constants of a Contact element, like FKN can -ve values be entered? ======================================= Answer: In the Real Constant menu, a negative value indicates an absolute value; and a positive is considered as a factor. So if FKN was specified as 0.1, its considered as 0.1*E Else, if FKN was specified as -2e10 then the value of FKN for the analysis is -2e10 %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 12. How does FTOLN affect convergence & Accuracy of results? ======================================= After FKN, FTOLN is the next parameter that affects both convergence & accuracy. Its usually known as Penetration Tolerance(TOLN) This is a factor of the depth of the underlying element. If the underlying elements depth was [h], and if FTOLN is specified as 0.1 (default value), a penetration of (0.1*h) is allowed. If this value was exceeded during the solution, then solution does not converge. Its aborted. In effect, this value can be treated as the Maximum allowable pentration. Setting too small a value can also affect in the form of excessive iterations or non-convergence. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 13. How and where is contact detected? ======================================= For STS elements, only the Target elements can penetrate into the Contact Elements and NOT vice-versa. Gauss-Integration points on the Contact Surface act as the Contact detection points. This is the default setting and is recommended for most cases. The Newton-Cotes/Lobatto nodal integration scheme, uses the Nodes of the Contact elements as Contact Detection points. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 14. There are several Contact Surface behaviour options on the Contact Wizard. What does each one of them do/describe? ======================================= STANDARD: Normal contact closing and opening behavior, with normal sticking/sliding friction behavior. ROUGH: Normal contact closing and opening behavior, but no sliding can occur. The surfaces are assumed to be so rough that there is infinite Friction and there can be no relative Sliding. BONDED: Target and contact surfaces are assumed to get GLUED once contact is established. BONDED CONTACT (always): Any contact detection points initially inside the pinball region or that come into contact are bonded for the remainder of the analysis. This contact typically can be used to "ADD" two meshes in a Assembly analysis where two parts have different meshes. A linear Static analysis can also be solved with this contact. Though ansys would prompt for nonlinear analysis(due to presence of contact elements) a single iteration is enough BONDED CONTACT (initial contact): Bonds surfaces ONLY in initial contact, initially open surfaces will remain open. NO SEPERATION: Target and contact surfaces are tied once contact is established (sliding is permitted). NO SEPERATION (always): Any contact detection points initially inside the pinball region or that come into contact are tied in the normal direction (sliding is permitted). %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 15. How should I simulate interference? Between two parts there exists both interference as well as Gap between their surfaces? Using STS Contact element, what factors need to be adjusted/set ? ======================================= In most of the FE models, the exact interfernce cannot be modeled with all that accuracy. Hence there exists a parameter called CNOF which can be tweaked, either to set a interfernce or a Gap. A positive value of CNOF is considered as INTERFERENCE, while a negative value of CNOF is considered as GAP. Using CNOF will either move the Contact Surface inwards/outwards for the Analysis. The Target surface will not be moved. So, if you are modeling contact btw two flexible bodies... please note that the surface designated as Target will not be offset. If the model contains initial geometric penetration+CNOF, it is recommended to set the initial interference option to "include with ramped effects". If this setting was not set, there is every chance that due to initial penetrations, the contact forces will be stepped (not ramped) to a huge value and there is every possibility for a un-converged solution. If both GAP and Interference exists in the model, different CNOF values will have to be specified between the various surfaces of the Parts. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 16. RIGID body motion error. I have the FE model with well defined constraints. Yet I see this error in the very beginning of the Solution. How can I avoid this error? ======================================= A rigid body motion can occur just before contact is established between two parts. You may use a displacement so as to initiate contact in the first load step. In the second load step delete this displacement, and apply the reaction force obtained from previous load step. This will switch your problem from displacement controlled problem to a force controlled problem. In the subsequent load step(3) continue with the load history. Weak springs that are connected to Ground can be used to control Rigid body motions. The Spring stiffness should be very small compared to the stiffness of the system. Though, the spring may deform... its of no concern. The above two techniques involve some experimentation from the user. Also, they cannot be used in all kinds of problems. They are restricted. Ansys provides 3 parameters to control RIGID BODY MOTION 1. ICONT 2. PMIN-PMAX and 3. CNOF 1. ICONT: This is a real-constant value, which specified a zone/band around the surface of Target Elements. Any contact points lying within this Zone, are shifted to the target surface. Ansys uses a small default value of ICONT if not specified by the user. This value should not be set to ZERO. If set to Zero, Ansys uses a default value. To turn it OFF specify a a very small value liek 1e-20. If there is a Gap of say 0.25mm between the Target and the contact surface & this happens to be the first place where contact happens, then specify ICONT as 10% more than this Gap. ICONT = 0.275mm Please note that ICONT is not any factor, its a constant value unlike other parameters 2. PMIN-PMAX: Use real constants PMIN and PMAX to specify an initial allowable penetration range. The Target surface shall be moved into the Contact Surface and made to lie within PMIN-PMAX. This is acheived with a few interations before the load history comes into effect. By using this feature, the gaps lying between Contact and Target Surfaces will be converted into a initial closed contact. If any of the nodes on the Target surface had constraints, then that particular node will not be moved in the constrained direction. 3. CNOF: [ see the previous FAQ. ] %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 17. In a Flexible-Flexible body contact, Why should the surface with finer Mesh be designated as Contact Surface, and the other surface (with coarse mesh) be designated as Target? ======================================= The Finer mesh will have more contact detection points. This will help the analysis solve better. Please note that elements/nodes on Target surface do not detect contact. In a flexible-flexible body contact, the choice of the target and contact surface can cause a different amount of penetration and thus affect the solution accuracy. Choose that surface which tends to move towards the other as the Contact Surface. (Assuming that both surfaces have same mesh density & have relatively small difference in their structural stiffness) %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 18. Guidelines to choose Target/Contact Surface ======================================= 1. If a convex surface comes into contact with a flat or concave surface, the flat or concave surface should be the target surface. 2. If one surface has a coarse mesh and the other a fine mesh, the surface with the coarse mesh should be the target surface. 3. If one surface is stiffer than the other, the stiffer surface should be the target surface. 4. If one surface is higher order and the other is lower order, the lower order surface should be the target surface. 5. If one surface is larger than the other, the larger surface should be the target surface %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 19. What is Pinball Region ? What does it affect? What is its purpose in Contact Analysis? ======================================= Pinball region (PIN<IMG src="http://okok.org/ut/images/smiles/smile_blackeye.gif" align=absMiddle border=0> affects the contact status determination. This Pinball Region is a circle (2D) or sphere(3D) around the Contact element. This Region helps figure out how "far" and "near" regions around the Contact element. If l ==> depth of underlying element, in Rigid-to-FLex Contact, the Pinball region is 4*l. For flex-flex contact, th Pinball Region is 2*l. The position and motion of a contact element relative to its associated target surface determines the contact element status. ANSYS monitors each contact element and assigns a status: STAT = 0 Open far-field contact STAT = 1 Open near-field contact STAT = 2 Sliding contact STAT = 3 Sticking contact A contact element is considered to be in near-field contact when its contact element enters a pinball region, which is centered on the integration point of the contact element. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 20. What type of Contact is best suited to simulate Interference fit kind of problems. ======================================= NTN type of Contact is best suited to simulate Interference Fit kind of problems. Most interference problems have negligible relative sliding deformation. NTN Contact is the least expensive in terms of solution times when compared to STS and NTS type of contact. Also, convergence issues are lesser. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% FAQ# 21. For NTN elements, how should the axis of NTN element be oriented? (I-J orientation of element) ======================================= Typically the I-J direction should be perpendicular to the contact surfaces. If the angles are not perpendicular undesired tangential responses will be generated between the Contact surfaces. %%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

laome · 发表于 2006-6-22 10:48

嗯不错啊 订上去！！！hoho！！

yxy910 · 发表于 2006-9-2 16:46

也支持一下1

zongzhou · 发表于 2006-9-2 17:21

怎么这么多符号啊，排版乱了点吧，不过还是谢谢了。

账号		自动登录	找回密码
密码			我要加入

[转帖]接触单元常问的问题及解答

马上注册，结交更多好友，享用更多功能，让你轻松玩转社区。

本帖被以下淘专辑推荐:

浏览过的版块