Week 4 -Wire Bending Challenge
OBJECTIVE
To carry out a static structural analysis on a wire bending simulation in ANSYS. The analysis will compare wires of the following non-linear materials - Copper Alloy, Aluminium Alloy and Magnesium Alloy. The analysis will be compared through outputs of the equivalent stress and strain generated on the wire.
MODEL IMAGE
PROCEDURE
Preface: After setting up and running the analysis in the first instance, all we need to do is change the material of the wire for each case.
1. After opening ANSYS Workbench, we are met with the Project Schematic window. Here, we can select the 'System Structural' analysis system on the left. Doing so creates a new project. Here, we can rename the project and also change the material if needed. We will need to right-click 'Geometry' and select 'import'. The file provided for this project should be selected.
Now, we can add the materials right here and make our job easier for later. To do that, we need to double-click Engineering Data'. This opens up the list of inserted materials. We can pick materials we need from the repository listed here. All of the materials we need (Aluminium Alloy NL, Copper Alloy NL and Magnesium Allow NL) are in the General Non-linear Material data source.
After that, we simply need to click the yellow '+' symbol on each material's corresponding 'add' column to add these specific materials to the project. Once we are done, we can simply close the tab.
We can then exit out of the engineering data tab and return to the project schematic window, where we can right-click geometry and select 'edit'. This will bring the model up in the Mechanical interface.
2. In the mechanical interface, in the outline, under geometry, we can rename each of the components if needed. We can rename them as 'wheel', 'wire' and 'lever' as shown. The material of the wire should also be assigned. The screenshot is of case 3 (Magnesium alloy wire).
3. We can then go to connections in the outline and right-click > rename based on definition. With this, we will know the location of each contact. We need to delete the contacts between the lever and the wheel & the wheel and the wire. That leaves the contact between the wire and the lever.
We can then duplicate the remaining contact and then flip it (one of the options that's available on right-clicking it). When we flip it, the wire surface becomes the target. We can then change the contact body - from the current lever surface to that of the wheel as shown (the curved surface is selected, except the surface directly opposite to the wire, which is marked by a circle).
Again, these changes are to be carried out on the duplicated contact. The original contact is to be left alone..
After that, we can select both contacts and assign the following settings:
4. Before we carry out the next step, we need to create a specific coordinate system on a certain region of the model. To create a coordinate system, we can simply right-click 'coordinate system' in the outline and select 'insert'.
With the new coordinate system selected, we are allowed to assign a geometry to it, for which we shall select the fillet region of the wheel, as shown in the screenshot. We can then add X and Z offset attributes to this coordinate system and assign the values 3mm and -3mm respectively.
5. We can then work on the mesh. Firstly, right-click mesh > insert > method. For 'geometry', select the entire model. The method would be 'tetrahedrons'.
Then, we can move on to sizing: right-click Mesh in outline > insert > sizing.
One instance of sizing will be used for the curved surface of the lever, the curved surfaces of the wire and just the fillet face of the wheel. Mesh size would be 2.2mm
The second instance will be a sizing with a sphere of influence type. The centre would be based on the coordinate system we created. The radius would be 7mm and the mesh size would be 0.8mm. The geomtery affected would be the wire surface only as shown:
6. Next, we shall work on the analysis settings. The number of steps would be 8. Selecting the 1st step only from the bottom toolbar, we can edit this particular step's properties in the entity window on the bottom left. Weak springs would be program-controlled and the solver type would be direct. The other highlighted settings should be edited as well:
For time steps 2 to 8, the Auto Time Stepping option would be 'on', it would be defined by time, the carryover time step would be on, Min. time step = 0.001s and Max. time step = 1.
For all steps, all the output controls should be enabled ('yes' should be selected).
7. We then need to create a revolute joint for the lever. The connection type would be body-ground. Also, for the coordinate system, we need to ensure that the z-axis points towards the wheel and the other axes are as shown in the following screenshot:
8. Next, we shall define the analysis settings. For that, we go to Static Structural > Analyses Settings. Right-click analysis settings > insert > fixed support.
We need to create two fixed supports - one would be the inner face of the wheel and the other would be the flat surface on the wire.
Fixed support geometries:
Next, we need to right-click static structural > Insert > Joint Load. We are to add a joint load for the revolute joint we created earlier on the lever. The type would be rotation and we need to create a displacement-time table with decrements of 20 degrees for each step as shown:
9. Now we can generate the outputs. To do this, we can right-click Solution > Insert > Strain > Equivalent (Von-Mises) (for equivalent strain) and right-click Solution > Insert > Stress > Equivalent (Von-Mises) (for stress). Each of these outputs will be solely for the wire body only (the geometry attribute of each output needs to specify the wire).
Now, all we need to do is right-click solution again and click 'Evaluate all results'. After the results are generated, we just need to save the project and come back to the mechanical interface and change the wire's material as per case requirement.
Care must be taken to ensure that the file is saved after generating the result in each case.
Finally, when the analysis is done, we can view the results by simply clicking each of these solution entities we created, in the Outline menu.
OUTPUTS
CASE 1 - COPPER ALLOY NL
Stress simulation with all parts active
Stress generated in the wire
Maximum/Minimum equivalent stresses generated in the wire
Strain generated in the wire
Maximum/Minimum equivalent strain generated in the wire
CASE 2 - ALUMINIUM ALLOY NL
Stress simulation with all parts active
Stress generated in the wire
Maximum/Minimum equivalent stresses generated in the wire
Strain generated in the wire
Maximum/Minimum equivalent strain generated in the wire
CASE 3 - MAGNESIUM ALLOW NL
Stress simulation with all parts active
Stress generated in the wire
Maximum/Minimum equivalent stresses generated in the wire
Strain generated in the wire
Maximum/Minimum equivalent strain generated in the wire
OBSERVATIONS
We can see that the highest amount of stresses are generated in the copper alloy wire but it experiences the least amount of strain on average. This explains the higher Young's Modulus exhibited by copper and its alloys in general, compared to those of aluminium and magnesium. This, coupled with its high ultimate strength, conductive and ductile properties, makes it ideal for usage as the material for wires.
From the outputs, we can see that most cases have the highest stress at the fillet of the wheel along which the wire is being bent. This is probably due to stress concentration as a result of the abrupt change in geometry along which the wire was being bent. In addition to that, the point of contact between the lever and the wire also generates comparable stress (probably as a result of stiffness), which explains why it's marginally higher in case 2.
RESULT
Thus, a structural analysis was carried out on the given wire which underwent bending. The required outputs of stress and strain generated on the wire were generated and compared for wires of different non-linear alloys of metals copper, aluminium and magnesium.