ABAQUS

1、界面数据显示框过小，数据无法看清怎么办？

解决办法：1）进入主菜单viewpoint选择Viewpoint Annotation Options

2)效果比较：

说明：主菜单中Viewpoint选项中还可以修改显示界面的形式，在模型上添加注释（Annotation），修改数据显示框的位置、大小、形式等等。

2、如何查看节点或单元在模型中的位置？

解决办法：1）在主菜单View栏下选中Toolbars，进而选中coustomize编辑框，选中“Group Display”则在主界面生成Group Display快捷操作框。

2）点击”create group display”进入对话框，可以查找相应编号的节点或单元在模型中的具体位置

3、分析结果中，显示的位移过大或者过小应该如何调整？

解决方法：在界面左边快捷栏点击“common options”

4、梁截面定义

** Section: Section-1-ADSET3 Profile: Profile-1

*Beam Section, elset=ADSET3, material=MATERIAL-2,temperature=GRADIENTS, section=L

0.12275, 0.12275, 0.007944, 0.007944 （a,b,t1,t2） -0.883444,-0.468537,0.

5、定义表面时“SNEG”“SPOS”表达的含义？

*Surface, type=ELEMENT, name=SURF-1 _SURF-1_SNEG, SNEG

*Surface, type=ELEMENT, name=SURF-1 _SURF-1_SPOS_1, SPOS

（SNEG/ SPOS的作用是什么？）

解答：Refers to the sides of the elements in the surface.用来指定选择的接触面。

EG:

6、RigidBody约束和刚体部件的差别在于：

刚体部件同部件相关联，RigidBody约束同组装实体中的区域相

关联。简单地讲，刚体部件建模时的整个部件在以后的分析中都将保持为刚体，而RigidBody约束可以是某一部件组装后的实体中的某一区域，相对刚体部件具有更高的灵活性。此外，刚体部件的参考点必须在Part模块下建立，Assembly模块下建立的参考点无法应用到刚体部件，但是RigidBody约束的参考点可以在Assembly模块下建立。 另外，值得一提的是，刚体部件可以在模型树中编辑修改为变形体，这一操作同增删RigidBody约束的作用是一致的。

Abaqus提供了多种不同的方式帮助用户简洁高效地进行刚体模

拟，包括： （1）离散刚体； （2）解析刚体； （3）RigidBody约束 ；

事实上，无论采用何种方式模拟刚体，只要在Abaqus中能够实现，其计算精度和效率都应该是接近的，因为在一个完整的模拟分析过程中，主要的计算精度和效率毫无疑问是由变形体所控制的，当然，不排除部分机构动力学分析中全部部件均采用刚体模拟的情形。但是，不同的刚体模拟方式还是具有一定差异的：

（1）离散刚体：离散刚体在几何上可以是任意的三维、二维或轴对称模型，同一般变形体是相同的，唯一不同的是，在划分网格时离散刚体不能使用实体单元，必须在Part模块下将实体表面转换为壳面，然后使用刚体单元划分网格。

（2）解析刚体：在计算成本上解析刚体要小于离散刚体，但是解析刚体不能是任意的几何形状，而必须具有光滑的外轮廓线。一般而言，如果可以使用解析刚体的话，使用解析刚体进行模拟是更为合适的。

（3）RigidBody约束：除了在Part模块下直接声明所建模型是离散刚体或解析刚体外，Abaqus在Interaction模块还提供了RigidBody约束用于模拟刚体性质。RigidBody约束实际上是将组装部件中某一区域的运动强制约束到参考点上，而在整个分析过程中不改变该区域内各点的相对位置。

7、部件生成以后，若需要更改部件的尺寸，应该怎么办？ 解答：在Part模块下，选择主菜单的“Feature” “Edit”,选择需要更改尺寸的部件，进行编辑。

通过“Edit Feature”编辑框，更改部件尺寸，而后点击“Feature” “Regenerate”，重新生成部件。

注意：重新生成部件以后，与部件对应的实体将会随之改变；但是重新生成部件以后，网格划分信息将会被删除！由inp文件导入的模型，无法用此方法更改部件尺寸。

8、

问题篇

1、出现错误“Error in job Job-freq: Three factorizations in a row failed. Check the model. It is possible that the model contains the kinematic coupling definition set up in a way that a degree of freedom has neither mass nor stiffness.”（三因子分解连续失败了。检查模型。有

可能模型包含运动学耦合定义设置,一个自由度既没有质量和刚度。）

解决办法：在求解结构动力特性时出现这类错误，最常见的一个原因就是没有定义结构自重或者结构重力定义不正确。 1）在Load模式下定义结构自重

2）在Step模式下，在动力分析前添加静力分析步

说明：检查结构自重加载是否正确的方法，即在加载重力的分析步中，结构是沿着重力方向变形的，如下图：（注意：结构自重设置是否正确，直接决定了结构动力特性计算的准确性）

2、出现错误“ERROR: TOO MANY ATTEMPTS MADE FOR THIS INCREMENT”，MSG文件中的警告信息“***WARNING: OVERCONSTRAINT CHECKS: NODE 4656 INSTANCE PART-1-1 ON THE SLAVE SURFACE AND CORRESPONDING NODE 17 INSTANCE PART-2-2 ON THE MASTER SURFACE HAVE EQUAL PRESCRIBED DISPLACEMENTS NORMAL TO THE CONTACT SURFACE. SINCE THIS MAKES THE CONTACT CONSTRAINT REDUNDANT, THE CONTACT STATUS AT THE SLAVE NODE IS CHANGED FROM CLOSE TO OPEN.

CONTACT PAIR (ASSEMBLY_SET-_CNS_,ASSEMBLY_SURF-1) NODE PART-1-1.3402 IS OVERCLOSED BY 31.8295 WHICH IS TOO SEVERE.”

解答： 这往往是因为接触面的法线方向定义反了。定义刚体和shell的surface时， 要注意选择外侧。

EG:对于这样一个导线与斜地面的接触问题，在定义地面接触面的时候会直观的将地面刚体的内侧面定义为接触面，从而导致错误； 由于地面是一个离散刚体，而刚体在定义surface时，只能选择外侧。故而，正确的做法是将外侧面即\"Purple\"面定义为地面与导线的接触面。

补充问题：对于下面的平地面接触问题，地面上侧和下侧是否均可定义为与导线的接触面？

解答是否定的，这种情况下只能选择“Brown”面作为与导线的接触面。

分别选择\" Brown \"和\"Purple\"面作为与导线的接触面，结果发现：选择\" Brown \"面作为接触面时，分析能够成功运行；而选择\"Purple\"面作为与导线的接触面时，分析不能成功，出现与上面相同的问题，即“CONTACT PAIR (ASSEMBLY_SET-_CNS_,ASSEMBLY_SURF-1) NODE PART-1-1.3402 IS OVERCLOSED BY 31.8295 WHICH IS TOO SEVERE.” 说明：平地面情况下，默认导线同侧的地面接触面为外侧面。

数据处理

1、origin中图层的使用方法：

在主菜单“graph”下，选择“layer management”进入图层管理编辑框，在这里可以添加或者删除图层，可以设置图层的大小（为方便比较，各图层易设置成同样大小）

在某一图层画图：首先，选中需要画图的数据；而后，点击绘图窗口中需要绘图的图层，在主菜单选中“graph” “add plot to layer”选择相应的线形就可在图层中绘制图形。

调整图层：新添加的图层往往会出现与原来图层错开的现象，如何调整？

首先，调整坐标轴，双击图形正，进入“layer property”编辑框，调整新图层坐标轴距

离左边及顶部的距离（调节为与旧图层相同的距离）；

然后，调节坐标轴数据，选中图层，点击坐标轴数据，调节数据和原图层一致（注意字体和大小也应和原图层一致）

附录1. 接触

1、Defining contact pairs in ABAQUS/Standard

After the selection of contact pair surfaces, three key factors must be determined when creating a contact formulation:

⑴ the contact discretization; ⑵ the tracking approach; and

⑶ the assignment of “master” and “slave” roles to the respective surfaces.

1.1 the contact discretization

ABAQUS/Standard offers two contact discretization options: a traditional “node-to-surface” discretization and a true “surface-to-surface” discretization. 1.1.1 Node-to-surface contact discretization

Traditional node-to-surface discretization has the following characteristics:

⑴ The slave nodes are constrained not to penetrate into the master surface; however, the nodes of the master surface can, in principle, penetrate into the slave surface

⑵ The contact direction is based on the normal of the master surface.

⑶ The only information needed for the slave surface is the location and surface area associated with each node; The direction of the slave surface normal and slave surface curvature are not relevant.Thus, the slave surface can be defined as a group of nodes—a node-based surface.

⑷ Node-to-surface discretization is available even if a node-based surface is not used in the contact pair definition

Fig.1 Node-to-surface contact discretization

1.1.2 Surface-to-surface contact discretization To optimize stress accuracy, surface-to-surface discretization considers the shape of both the slave and master surfaces in the region of contact constraints. Surface-to-surface discretization has the following key characteristics: ⑴ Contact conditions are enforced in an average sense over the slave surface, rather than at discrete points (such as at slave nodes, as in the case of node-to-surface discretization). Therefore, some penetration may be observed at individual nodes; however, large, undetected penetrations of

master nodes into the slave surface do not occur with this discretization. ⑵ Surface-to-surface discretization is not applicable if a node-based surface is used in the contact pair definition. 在某一个迭代步中,面对面的接触计算成本一般较点对面的接触的计算成本高,但多数情况下这个成本不会高很多,只有在下列情况下才会让计算成本急剧增大: ⑴ 模型的绝大部分区域被包含于接触中; ⑵ 当主动面比从属面网格划分还要精细时; ⑶ Multiple layers of shells are involved in contact, such that the master surface of one contact pair acts as the slave surface of another contact pair.

尽管如此,但点对面的接触需要花费更多的迭代步才能达到数值稳定,从某种意义上来说,在一个分析步中,无法判定到底是用点对面接触还是面对面接触计算成本低.

1.2 Contact tracking approaches

In ABAQUS/Standard there are two tracking approaches to account for the relative motion of the two surfaces forming a contact pair in mechanical contact simulations:

⑴ The finite-sliding tracking approach ⑵ The small-sliding tracking approach 1.3 Fundamental choices affecting the contact formulation

Your choice of contact discretization and tracking approach have considerable impact on an analysis. In addition to the qualities already discussed, certain combinations of discretizations and tracking approaches have their own characteristics and limitations associated with them. These characteristics are summarized in Table 1. You should also consider the solution costs associated with the various contact formulations

Table 1 Comparison of contact formulation characteristics

1.4 选择主动面和从属面的几个原则

⑴ Analytical rigid surfaces and rigid-element-based surfaces must always be the master surface. ⑵ A node-based surface can act only as a slave surface and always uses node-to-surface contact. ⑶ Slave surfaces must always be attached to deformable bodies or deformable bodies defined as rigid. ⑷ Both surfaces in a contact pair cannot be rigid surfaces with the exception of deformable

surfaces defined as rigid 一般来说,当定义两个基于单元的面作为解除对作用面时,当存在一个较小的面和一个较大的面时，一般将较小的面定义为从属面。当两个面大小接近时，选取较“硬”的面或单元划分笔记粗糙的面作为主动面。值得注意的是，“硬”的面不一定是材料弹性模量大的材料，比如当一个薄金属片和一个橡胶材料接触时，此时就应该将薄金属片所属的面定义为从属面。当两个面区域接近，“硬度”也接近时，此时往往需要反复尝试才能得到较好的结果。 与点对面接触相比，面对面接触中主动面和从属面的选取，对计算结果的影响并不是很大。但是，当错误的将网格粗糙的面定义为从属面时，此时也许会引起计算成本的急剧增加。

1.5定义接触对

为了定义一个接触对，必须指定一对接触面或者一个自接触的面，一个contact formulation。每一个接触对可以定义不同的作用面性质。 1.5.1 Defining contact between two separate surfaces When a contact pair contains two surfaces, the master and slave surfaces are not allowed to include any of the same nodes and you must choose which surface will be the slave and which will be the master. ABAQUS/Standard定义接触默认采用的是有限滑移、点对面接触。如果定义的是小滑移，默认的也吃采用点对面接触。

1.5.2 用对称的主从接触对提高接触模拟精度 对于点对面接触，主动面上的节点很容易penetrate到从属面上去，此时，提高从属面上单元的网格划分精度，有助于减少这样的刺入，提高运行速度。才外，让两个面都是基于单元定义时，可以用symmetric master-slave method。To use this method, define two contact pairs using the same two surfaces, but switch the roles of master and slave surface for the two contact pairs. This method causes ABAQUS/Standard to treat each surface as a master surface and, thus, involves additional computational expense because contact searches must be conducted twice for the same contact pair. The increased accuracy provided by this method must be compared to the additional computational cost. All of the contact formulations are available for symmetric master-slave contact pairs, and can be applied using the same options discussed above. 命令语句如下： *CONTACT PAIR, INTERACTION=interaction_property_name

surface_1, surface_2 surface_2, surface_1

1.5.2.1 对称主从接触结果的解释 对于单一的主从接触，输出结果仅对从属面输出。而对称主从接触，每一个面都是从属面，均输出计算结果。问题在于，两个从属面上的接触压力并不是相对的，也并不一定相等，总的接触压力为两个面上的接触压力之和。

1.6给接触对赋予接触面定义

命令语句如下：

*CONTACT PAIR, INTERACTION=interaction_property_name *SURFACE INTERACTION, NAME=interaction_property_name

1.7 选择接触面

除了小滑移、面对面接触之外，主动面必须为单一面。 三维梁单元、桁架单元，不能用来作为主动面，但却可以定义为从属面。二维梁单元、桁架单元可以定义为主动面或从属面。

Edge-based surfaces on three-dimensional shell elements cannot be used in a contact analysis in ABAQUS/Standard.

1.8 结果输出

You can write the contact surface variables associated with the interaction of contact pairs to the ABAQUS/Standard data (.dat), results (.fil), and output database (.odb) files. All contact pair results are given at the constraint points of the slave surface. The constraint points correspond to the slave nodes except in the case of finite-sliding, surface-to-surface contact, in which case each slave facet contains multiple constraint points. You can: ⑴ request output associated with a given contact pair;

⑵ request output associated with a given slave surface, including contributions from all of the contact pairs to which the slave surface belongs; and

⑶ limit the output by specifying a node set containing a subset of the nodes on the slave surface except in the case of finite-sliding, surface-to-surface contact. 下面为常用的接触输出语句：

*CONTACT PRINT, SLAVE=SURFNAME, MASTER=SURFNAME, NSET=NODESET 以下为输出到.dat文件的结果形式：

对于结果的解释： ⑴ This output request creates a table of output variables in the printed data (.dat) file. Each row of the table corresponds to a slave node in node set SNODES. The first column of the table identifies the slave node for that row. Because this is a mechanical contact simulation, the second column specifies the contact status at the slave node. Since the contact property definition includes frictional properties, the contact status may be open (OP), closed and sticking tangentially (ST), or closed and sliding tangentially (SL). The remaining columns contain the surface variables requested. In this example the default variables—contact pressure, contact opening, frictional shear stress, and relative tangential slip—were requested. ⑵ The OP status indicates that the slave node is not in contact with the master surface. In the sample output above, node 101 is open and, consequently, the contact pressure variable CPRESS is zero. The COPEN variable reports that this node is 0.66 length units away from the master surface. ⑶ The ST status indicates that the slave node is in contact with the master surface and is “sticking.” The frictional shear stress acting at the node is below the critical shear stress , where p is the value of contact pressure shown under CPRESS. In the sample output above, node 102 is sticking since the frictional shear stress CSHEAR1 is below the critical value of 2. (0.4 × 6.59). The CSLIP1 variable is the total accumulated (integrated) slip at the slave node. The negative magnitude of CSLIP1 indicates that the node has moved in the negative first slip direction on BSURF. Accumulated slip and slip directions are discussed in more detail below in “Output of tangential motion of the surfaces.” ⑷ The SL status indicates that the slave node is in contact with the master surface and it is sliding—the frictional shear stress is at the critical shear stress ==. In the sample output above,

node 103 is sliding, and the frictional shear stress CSHEAR1 is equal to the friction limit 1.73 (0.4 × 4.32). ⑸ In the absence of frictional properties when a slave node is in contact with the master surface, its status reads CL for “closed.”

2、Modeling contact interference fits in ABAQUS/Standard

2.1 Resolving excessive initial overclosures

3、ABAQUS/Standard中接触模拟的常见错误

3.1 解决初始接触的错误

3.1.1 消除初始的过盈接触和张开 当两个不同Part的面接触时，由于单元网格不一致，很可能会在两个面之间留下小的gap或penetration。默认的，ABAQUS/Standard会将初始penetration当成interference fits，并会相应地在接触一开始的时候处理掉，见“Modeling contact interference fits in ABAQUS/Standard,” Section 29.2.4. 计算中必须通过调整从属面位置来提高接触模拟精度，以保证接触刚开始时计算中没有penetration。当初始的clearance或overclosure与单元典型尺寸相比较小时，在小滑移接触模拟中，你可以精确的指定clearance或overclosure，以消除初始的过盈接触和张开，见“Adjusting the surfaces in a contact pair” in “Adjusting initial surface positions and specifying initial clearances in ABAQUS/Standard contact pairs,” Section 29.2.5. 3.1.2 消除刚体位移 动力分析中刚体位移不会引起数值奇异问题，但在静力问题中，当一个体没有给予足够的约束时，将会引起刚体位移，从何会引起数值奇异问题和大位移（“Numerical singularity” warning messages and very large displacements） 可以通过指定该体的边界条件，或用弹簧或阻尼器将该体接地，以消除刚体位移。 如果不能通过上述办法消除刚体位移，ABAQUS/Standard还会提供一些工具，可以在接触模拟过程中，自动的解决刚体稳定性问题。见“Automatic stabilization of rigid body motions in contact problems” in “Adjusting contact controls in ABAQUS/Standard,” Section 29.2.12.

3.1.3 解决过大的interference fits ABAQUS/Standard interprets initial overclosures as interference fits, which it tries to resolve in the first increment of a step. If the initial overclosures are an unintended result of mesh discretization, you should use one of the methods discussed above to remove the overclosures. In some cases the interference fit may be intended but too large for ABAQUS/Standard to resolve in a single increment. In this situation you should redefine the interference fit to allow resolution of the overclosures over multiple increments. See “Modeling contact interference fits in ABAQUS/Standard,” Section 29.2.4, for more information.

3.2 低精度表面（Poorly defined surfaces）

粗糙的网格、不合适的单元和过度扭曲的表面形状，均可导致接触计算的中止。 3.2.1 主控面定义重复节点 三维有限滑移接触分析中，应避免用相同坐标的节点定义不同的surface，这样的定义容易引起接缝或裂缝（seam or crack）。

虽然从CAE默认的视角来看，这个定义的面仍然是一个连续有笑的面，但当接触计算开始时，从属面上的点很可能滑落到这个seam or crack中去，使得从属面上的某些节点被黏附在主控面后面，从而引起计算的中止。类似的情况也会出现在finite-sliding, surface-to-surface contact。

3.2.2 避免沿表面边界的接触问题 有限滑移接触分析中，主控面必须定义得足够大，以至于可计算接触分析中所用可能存在的位移。如果主控面定义不恰当，从属面上的从属点很可能在迭代计算过程中滑落到主控面后面，引起振颤问题（chattering）。 当计算过程中出现振颤问题时，msg文件中会有一个或几个从属点不停的循环出现闭合和张开，此时，可在关键词*Contact Pair中实用参数Extension Zone来扩大主控面的尺寸，具体见“Extending master surfaces and slide lines,” Section 29.2.8.

3.2.3 面单元网格粗糙 如果面单元网格太粗糙，将会发生以下几个问题： ⑴ 主控面刺入从属面过多 在点对面接触中，当从属面单元网格过于粗糙，以至于主控面会很严重的刺入到从属面中去时，将会引起错误，此时应细化从属面单元网格。 对于面对面接触，虽然这种接触模式会有效抵制主控面刺入到从属面中，但当从属面网格比主控面还要粗糙时，此时的计算成本将会变得非常大。

3.3 接触模拟中的过多迭代

ABAQUS/Standard提供了一些方法，可以调整接触模拟迭代过程，以提高计算效率，并不影响计算精度。

3.3.1 Converting severe discontinuity iterations in weakly determined contact conditions ABAQUS/Standard对规则平稳的迭代和严重不连续迭代加以区分。最普遍的严重不连续现象有张开－闭合转变和静止－滑移的摩擦面行为转变。 在两种情形下，默认的算法会导致收敛问题或过多的小增量步。第一种情况是接触定义不明确。例如，在冲压问题中，冲头与薄片在边界上发生接触，但冲头中心处定义并不明确。典型的，该点处于接触状态时，接触压力会很小；当该点没有处于接触状态时，其张开距离也会很小。这就会引起振颤问题。 第二种情况是大接触问题，即一个模型中存在很多接触点（或接触对）。在此种情况下，ABAQUS会经过多次迭代来判定其初始接触条件（因为每一次迭代会有不同的接触点其接触状态发生变化，或张开、或闭合）。默认的情况下，

3.3.2 Controlling the increment size based on penetration distance in unconverged iterations

多数接触迭代计算过程中，如果penetration超过了指定的距离hcrit，ABAQUS/Standard就会放弃当前增量步，而尝试一个更小的增量步。对于有限滑移、面对面接触和几何线性小滑移分析，并没有严格的hcrit距离规定。

默认情况下，hcrit等于通过单元表面几何体的半径。在下面几类情形中，有必要修改hcrit⑴ 主控面高度扭曲。如图，在迭代过程中，从属面节点b有可能落入到主控面，相当距离值：

于从属节点penetration主控面，overclosure 即h，小于hcrit。此时迭代过程会尝试将节

点b移动到主控面上的投影c点处。为了避免此类迭代，可尝试指定一个较小的hcrit，强迫ABAQUS/Standard放弃当前操作，而尝试一个较小的增量步。

⑵ a node-based surface在接触面中存在时，ABAQUS/Standard将会无法计算得到一个

合理的hcrit。当存在其它面接触队时， ABAQUS/Standard采用从属面上单元的average dimension作为hcrit。如果没有其它接触对存在，ABAQUS/Standard将采用整体模型的a characteristic element dimension。

⑶ 从属面形状变化剧烈

⑷ 软接触中允许较大的penetration。 命令语句如下：

*CONTACT PAIR, HCRIT=hcrit

4、Extending master surfaces and slide lines

延伸主控面或滑移线，可以： ⑴ 在有限滑移问题中，可以避免从属面节点落入或滑道主控面背后； ⑵ 在小滑移问题中，当主控面与从属面没有相接时，可以保证从属面节点能在主控面上找到一个投影点； ⑶ 能避免一些接触模型中数值计算问题； ⑷ 不能用来代替正确的接触； ⑸ 不能用来减少接触面下的单元数目（surface based on element） ⑹ 仅适用于点对面接触（node-to-surface discretization）

For node-to-surface contact you can specify the size of the extension zone, e, as a fraction of the end segment or facet edge length (see Figure 29.2.8–2). If e is set to zero, ABAQUS will not extend the ends. The value given must lie between 0.0 and 0.2. The default value is 0.1 for node-to-surface contact; surface extensions are not available for surface-to-surface contact。

命令语句如下： *CONTACT PAIR, SMALL SLIDING, EXTENSION ZONE=e

5、调整接触控制

接触控制在ABAQUS/Standard中：

⑴ 不能用于修改多数接触问题的默认接触属性设置； ⑵ 可用于计算过程中未提供有效收敛控制的接触算法； ⑶ 可用于未建立有效接触模拟过程中。

6、Abaqus/Standard中General Contact和Contact Pairs的异同及选择

对于大多数的接触问题，在ABAQUS中有通用接触（General Contact）和接触对（Contact Pair）两种算法处理，它们的异同主要体现在用户交互、默认设置、可选设置三个方面。

总的来说，通用接触算法的相互作用主体、接触属性、接触面属性是可以各自地指定，它提供了一个更有弹性的方法去增加模型中接触的细节。通用接触算法允许非常自动化的接触定义，尽管也可以采用传统的、类似于接触对算法的方法去交互式定义。对于传统的接触对算法，相对于全部包括式的自接触（Self-contact），接触对算法的计算效率可能更高，而且使用CAE也能比较方便地建立接触对。因而这两种接触算法的选择其实就是一个在接触定义的便利性和计算效率性之间的平衡，它们之间的差异主要有：

一、通用接触（General Contact）和接触对（Contact Pair）的默认设置差异

1、接触离散方式：通用接触算法使用有限滑动和面对面的离散方式，而接触对算法使用有限滑动和点对面的离散方式；

2、对壳的厚度和偏移的处理：通用接触算法自动考虑，接触对算法在使用点对面的离散方式时不考虑壳的厚度和偏移；

3、接触的执行：通用接触算法采用罚函数方法，接触对算法在使用点对面的离散方式时采用拉格朗日乘数方法；

4、初始过盈量的处理：通用接触算法采用无应变调整的方法消除过盈量，接触对算法将过盈量作为穿透在第一个分析增量步处理；

5、主从面指定：通用接触算法自动指定，接触对算法必须由用户指定。 当接触对算法采用有限滑动和面对面的离散方式时，就没有前三个差异了。 二、可选的接触属性

下列功能只有接触对算法拥有：

1、包含RSURFU子程序定义的刚性面或解析刚性面的接触，当然基于单元的刚性面通用接触和接触对都可以；

2、包含基于节点的面或者三维梁单元面的接触； 3、小滑移接触和绑定接触；

4、有限滑动和点对面的离散方式； 5、粘性接触； 6、压力渗透加载；

7、粗糙摩擦模型（Rough）； 8、用户子程UINTER和FRIC；

9、Lagrange enforcement of friction constraints；

10、Local definitions of some numerical contact controls 注：同一个模型可同时使用通用接触算法和接触对算法。Explicit中的异同参考AUUM 31.1.1

7、Element-based surface definition

7.1Defining single-sided surfaces

You can define a single-sided surface on the positive or negative face of

structural, surface, or rigid elements. The positive face is defined as the one in the direction of the positive element normal, and the negative face is defined as the one in the direction opposite to the element normal. The definition of the element normal for all elements is given in Part VI, “Elements.”

You must ensure that all of the specified elements have their normals oriented consistently. If they are oriented as shown in Figure 2.3.2–4, the surface

normals will reverse direction as the surface is traversed and improper results may occur when the surface is used with features requiring an orientation such as distributed surface loads.

Figure 2.3.2–4 Inconsistent orientation of structural element normals can result in an invalid surface.

Further, an error message will be issued and the analysis will terminate if this condition is detected for surfaces used with mesh tie constraints in Abaqus/Standard or with contact pairs. To correct the surface orientations in this figure, two separate element sets with different face identifiers should be used.

Input File Usage: Use the following option to define a surface on the positive face

of a structural, surface, or rigid element:

*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, SPOS

Use the following option to define a surface on the negative face of a structural, surface, or rigid element: *SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, SNEG

For example, single-sided surfaces on the positive faces of the elements in element setSHELL can be defined using input similar to

*SURFACE, NAME=BSURF, TYPE=ELEMENT SHELL, SPOS

Abaqus/CAE Usage: Any module except Sketch, Job, and

Visualization: ToolsSurface

Create: Name:surface_name, pick face in viewport, click mouse button 2, and specify the side of the selected face

(说明：SPOS, 是Surface-Positive的缩写；SNEG, 是Surface-Negative缩写)

7.2Defining double-sided surfaces

You can create double-sided surface facets on three-dimensional shell, membrane, surface, and rigid elements using the automatic surface facet

generation approach (i.e., specifying only the element numbers or sets). Some applications that refer to surfaces do not allow the use of double-sided surfaces: examples include contact pairs in Abaqus/Standard and features requiring an oriented surface such as distributed surface loads. When

double-sided surfaces can be used, they are often preferred to single-sided surfaces. In some applications, such as when defining the contact domain for general contact, it does not matter whether single- or double-sided surfaces are used.

When double-sided surfaces are used with contact pairs in Abaqus/Explicit, the normals of all the underlying elements do not need to have a consistent positive orientation: Abaqus/Explicit will define the contact surface such that its facets have consistent normals, even if the underlying elements do not have consistent normals. The facet normals will be the same as the element normals if the element normals are all consistent; otherwise, an arbitrary positive orientation is chosen for the surface. The positive orientation is

significant only with respect to the sign of the contact pressure output variable for the contact pair algorithm, CPRESS (see “Output” in “Defining contact pairs in Abaqus/Explicit,” Section 32.5.1).

Although contact is enforced unconditionally on both sides of a surface when self-contact is used with contact pairs, contact is enforced on both sides of a surface used in two-body contact only when that surface is double-sided (if allowed). The use of single-sided surfaces with contact pairs is sometimes desirable: the resolution of large initial overclosures in contact pairs is more robust with single-sided surfaces than with double-sided surfaces

(see“Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 32.5.4). However, single-sided contact is generally more limiting than double-sided contact; it may cause an analysis to fail due to excessive element distortion or not enforce the contact conditions realistically if a slave node unexpectedly moves behind a master surface. This condition can occur, for example, when large deformations or rigid-body motions are present or due to complex tool shapes in a forming analysis.

Input File Usage: Use the following option to define a double-sided surface on

three-dimensional shell, membrane, surface, or rigid elements in Abaqus/Explicit:

*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set,

For example, double-sided surfaces on the elements in element set SHELL can be defined using input similar to *SURFACE, NAME=BSURF, TYPE=ELEMENT SHELL,

Abaqus/CAE Usage: Any module except Sketch, Job, and

Visualization: ToolsSurface

Create: Name:surface_name, pick face in viewport, click mouse button 2, and choose Both sides

7.3Defining edge-based surfaces

You can define an edge-based surface on three-dimensional shell, membrane, surface, or rigid elements by specifying the individual edges. Alternatively, you can specify that all the edges of the elements that are on the exterior (free) surface of the model are used to form the surface; this method cannot be used to define edge-based surfaces that are in the interior of the model. It is

possible to use both methods in the same surface definition when creating a single surface.

Input File Usage: Use the following option to specify the individual edges that form

the surface:

*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, edge identifier

The individual edge identifiers used in Abaqus are listed in Table 2.3.2–2.

Use the following option to specify that all the edges of the elements that are on the exterior (free) surface of the model are used to form the surface:

*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, EDGE

For example, if the shaded element set in Figure 2.3.2–2 is composed of three-dimensional shell elements and is named ESETA, the surface named ESURF could be specified by the following input: *SURFACE, NAME=ESURF, TYPE=ELEMENT ESETA, EDGE

Abaqus/CAE Usage: Any module except Sketch, Job, and

Visualization: ToolsSurface

Create: Name:surface_name, pick edges in viewport

In Abaqus/CAE you can specify that all the edges of the elements that are on the exterior (free) surface of the model are used to form the surface by directly picking all the free edges in the viewport.

7.4Defining a surface over the cross-section at the ends of beam, pipe, and truss elements

To define a surface over the cross-section of beam, pipe, or truss elements, you must specify the end on which the surface is defined. Surfaces created on the ends of these elements can be used only for integrated output request (see “Integrated output in Abaqus/Explicit” in “Output to the output database,” Section 4.1.3) and integrated output section (see “Integrated output section definition,” Section 2.5.1) definitions.

Input File Usage: Use the following option to define a surface over the

cross-section of a beam, pipe, or truss element:

*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set, END1 or END2

Abaqus/CAE Usage: Any module except Sketch, Job, and

Visualization: ToolsSurface

Create: Name:surface_name, pick three-dimensional wire region in viewport, click mouse button 2, and choose End (Magenta) or End (Yellow)

Defining a surface along the length of three-dimensional beam, pipe, and truss elements

You cannot specify the faces to define a surface along the length of

three-dimensional beams, pipes, or trusses because their element connectivity cannot define a unique element or surface normal. Instead, you must specify that Abaqus should generate a surface for these elements. Therefore, the use of surfaces along the length of these elements is restricted.

In Abaqus/Standard element-based surfaces created along the length of

three-dimensional beam, pipe, or truss elements can be used in tie constraints but can be used only as slave surfaces in contact interactions. However, there are several advantages to using an element-based surface rather than a node-based surface when modeling contact in Abaqus/Standard with three-dimensional beams, pipes, or trusses:

1. The default slip directions are parallel and orthogonal to the element axis.

2. Abaqus/Standard calculates the contact results as contact forces per unit length rather than just contact forces.

3. It can be easier to define an element-based surface than a node-based surface.

In Abaqus/Standard a surface definition is not allowed for cases where three or more three-dimensional beams, pipes, or trusses are joined at a common node because of the lack of uniquely defined element tangents.

In Abaqus/Explicit element-based surfaces created along the length of three-dimensional beam, pipe, or truss elements can be used only with the general contact algorithm or tie constraints. To define contact for these

elements using the contact pair algorithm, the nodes forming the beam, pipe, or truss elements can be included in a node-based surface definition

(“Node-based surface definition,” Section 2.3.3) and a contact pair can be defined for this node-based surface and a non-node-based surface. Surfaces along the length of three-dimensional beam, pipe, or truss elements cannot be used to prescribe a distributed surface load since the loading direction is not unique.

Input File Usage: Use the following option to define a surface along the length of a

three-dimensional beam, pipe, or truss element:

*SURFACE, NAME=surface_name, TYPE=ELEMENT element number or element set,

Abaqus/CAE Usage: Any module except Sketch, Job, and

Visualization: ToolsSurface

Create: Name:surface_name, pick three-dimensional wire region in viewport, click mouse button 2, and choose Circumferential

附录2. 输电塔输出节点单元位置

ZXY

图.输出节点的位置标识

图.主要分析杆件位置图

图.绝缘子位置

图.输出线单元的位置