	Department of Engineering

University of Cambridge > Engineering Department > computing help

The MSC/PATRAN FAQ

6. Finite Elements

Q6.1 : The f.e. mesh I have created has many more elements than I had expected. What do I do?

This usually happens due to sides which have not been assigned mesh seeds. On these sides Patran uses the Element length (L) to work out how many elements should be generated along the side. Click on the `Element Length' button and this will display the current setting.

Click on the button marked Display Existing Seeds to find out which sides have not been assigned seeds. Specify the mesh seeds along which many elements were generated. Then delete the current finite element mesh and re-generate it.

To delete the current mesh change the Action to Delete and then select the finite element mesh by drawing a box around the whole mesh.

Q6.2 : What do I do to get the current mesh seeds displayed?

In the Finite Elements form choose the following :

Action :  Create
Object :  Mesh seed
Type   :  Uniform

Then click on the label Display Existing Seeds. This should display the current seeds. The number of yellow circles along each side represnts the no. of divisions.

Q6.3 : How do I go about assigning mesh seeds differently to different parts of the geometry? It seems tedious if the geometry is complex and has many surfaces?

You can hold down the Shift key when clicking on the sides. This allows you to make multiple selection.

Opposite sides of the surfaces are meshed identically. The following figures show the minimum number of sides for which the mesh seeds have to be specified.

Can you figure out why the 3 curved sides along the outer boundary (denoted by X) have not been assigned any mesh seeds?

Q6.4 : When making copies of surface already assigned mesh seeds does the information about the mesh seeds 'remembered' by the copies?

No.

Q6.5 : How do I add a concentrated mass?

Click on radio button Finite Elements and in the form make the following selection :

Action : Create
Object : Element
Method : Edit

Shape : Point

Then click on the node where you want to position the concentrated mass and then click on Apply. It should display a red triangle at this node.

Then click on the radio button Properties and in the form make the following selection :

Action : Create
Object : 0D
Method : Mass

In the box marked Property Set Name anter a name for the concentrated mass. Then click on the button marked Input Properties... and enter the mass of the element in the box marked Mass Magnitude and click on the OK button. In the original form click on the Select Members input field. Select the Point Element icon from the `Select Menu' and then click on the element created before (red triangle). Then click on Add and finally on Apply.

Q6.6 : I am trying to create a `Beam is Space' for use with ABAQUS and I am getting the following error message?
A Value for Property "Definition of XY Plane" must be entered. Check the remaining property values.

In the form that comes up when you click on Input Properties... in the Properties form you need to enter the gradient of the in the 1-direction in the box marked Definition of XY Plane. Enclose this in angled brackets. For example if the beam cross-section is rectangular as shown below :

Consider the 3 beams spreading out from a point radially (see plan view shown below). If each is of rectangular section then the gradient in 1-direction is as shown. This is the data that should be entered in the box marked Definition of XY Plane.

Even if the cross-section is circular you need to specify a direction for the above category.

Q6.7 : I am trying to create shell elements using the `Finite Element' form. The only choice I can make is the order of the element : Quad4, Quad8. What needs to be done?

At this stage just choose the appropriate order for the element. Example : Quad4 or Quad8.

Then in the form Properties choose the following options :

Action    : Create
Dimension : 2D
Type      : Shell

This will select the required shell elements. However if you require elements for Plane stress or Plane Strain then change the Type to 2D Solid.

Q6.8 : The geometry I have created is dividied into different groups. I want to create a new single group (say called `fem') to receive all the finite elements that will be generated. How do I do that?

Click on the pull-down menu Group and select the option Create.... In the form that pops in the box marked New Group Name enter an appropriate name (say fem and then click on the Apply button. Then click on the Cancel button to close that form. This will create the new group to receive the finite element mesh.

Click on the pull-down menu Group and this time select the option Post.... In the form that pops in the box marked Select Groups to Post click on the newly created group ( fem ) and click on the Apply button. You will notice the viewport cleared and the heading changing to the new group name.

Then holding down the Ctrl key select all the groups which contains the geometries (by clicking the left mouse button). Then click on Apply.

This should display all the geometries in the viewport. However the viewport heading should still be the name of the group created for the finite elements.

Now click on the radio button Finite Elements and assign mesh seeds to the side and create the mesh. Once the mesh has been created and click on the pull-down menu Group and select the option Post.... In the form that pops in the box marked Select Groups to Post click on the newly created group ( fem ) and click on the Apply button.

Now only the newly created finite element mesh should be on display (and none of the geometries).

Q6.9 : Is it possible to assign mesh seeds at points which do not follow the uniform / one way bias / two way bias options?

Yes there is a further option which allows one to assign mesh seeds at precisely the points at which these are needed. This is done using the Tabular option. Here the locations of the seeds are worked out in fractions w.r.t the length of the side and these are entered in a table.

Q6.10 : Can equivalencing be used to join the nodes from 2 different parts (of an assembly) created and imported from Pro/ENGINEER?

It is possible but not recommended. Because it is unlikely that the position of the nodes will coincide in the contact surface from the 2 sides. Equivalencing under these circumstances will only remove duplicate nodes which match from both sides. This will leave all other nodes which do not coincide. This will be unsatisafctory if the coincident nodes are very few.

If using ABAQUS it is preferrable to define a contact pair and then use the option TIE then it will have the same effect as applying equivalence if all the nodes in the contact surface were coincident.

Q6.11 : Is it possible to create an unstructured 2-dimensional mesh?

Yes it is possible to create an unstructured mesh using the paver option. In the Finite Elements form choose : Action / Option / Type = Create / Mesh / Surface. Then choose the radio button Paver instead of Isomesh.

Similarly for 3-dimensional mesh choose Tetmesh instead of Isomesh.

Q6.12 : Is it possible to create an unstructured mesh made up of quadrilateral elements?

Yes it is possible to create an unstructured mesh consisting of quadrilateral elements.

See the answer to the question Q6.11.

Q6.13 : I have imported a cylinder (as part of an assembly) from Pro/ENGINEER but I cannot mesh it using brick elements. Why is that?

Yes. It is not possible to mesh a cylinder into brick elements if the cylinder was created in Pro/ENGINEER. The reason is that any object created in Pro/ENGINEER whether it be a cylinder or rectangular solid are "General Trimmed Surfaces" and these are coloured Magenta. These solids can only be meshed with the option 'tetmesh' ie tetrahedras.

| Computing Help |[Finite Elements] | [Engineering Packages]