PDF
Deformation of a Feeder Clamp
Introduction
This example, from the field of structural mechanics, analyzes the deformation of a feeder clamp under stress. The clamp secures a feeder that carries high-frequency electromagnetic fields, and it’s important that it remains as straight as possible.
This example analyzes deformations in the clamp with the following questions in mind:
•
How much does the force from the feeder incline the clamp? The inclination must be less than 1 degree.
•
Does a prestressed screw of a certain type have enough strength to deform the clamp so that it adequately anchors the feeder? The gap must shrink by at least 0.5 mm.
•
What happens if one of the mounting bolts is loose or missing?
Model Definition
In this analysis, the feeder clamp is bolted to a wall. The fastening can be made using either one or two mounting holes. The mounting using two holes represents a case when the fastening is properly made while fastening using only one hole represents a case when the clamp is poorly secured. The external forces on the clamp are introduced from the feeder as well as from the clamping screw, as shown in Figure 1.
.
Figure 1: Applied forces.
Loading Data
The clamp is made of aluminum. Assume that an installation technician fastens the feeder into the clamp using a standard metric M3 screw of Class 8.8 (where the first digit stands for a breaking load of 800 N/mm2, and the second digit indicates a yield strength of 80% of the breaking strength). Prestressing the screw to the yield limit results in a screw force of 4500 N. This application tests if a screw force of 20% of this value is adequate. A 7-mm washer distributes the prestressed load evenly onto both sides of the sleeve. The maximum load from the feeder onto the clamp is 2000 N, and is applied evenly throughout the inner surface of the sleeve.
Due to symmetry in both loading and the geometry, you can perform a complete model analysis while looking at only one half of the geometry. For illustrative purposes though, this example models the entire geometry.
Results and Discussion
The deformation of the loaded clamp when secured with two bolts is shown in Figure 2. In Figure 3 the deformation is shown when fastening is made using only one bolt. The results indicate clearly a larger deformation when one fastening element is missing.
Figure 2: Displacement of the clamp in the loading direction in case of two mounting bolts.
.
Figure 3: Displacement of the clamp in the loading direction in case of only one mounting bolt.
Since the problem is symmetric in the yz-plane the minimum separation of 0.5 mm can be visualized by evaluation of the expression abs(u)  >  0.25 mm, shown in Figure 4. The non-green color marks domains that experience a greater displacement than 0.25 mm which due to symmetry marks part of the clamp that undergoes a larger deformation than 0.5 mm, which is the minimum requirement for being able to fasten the feeder adequately. The boundary conditions in this example are valid only as long as the installation technician does not squeeze the gap in the clamping sleeve completely shut. However, if the gap is squeezed shut, you can be sure that the requirements are fulfilled.
Figure 4: Clamp deformation caused by the screw force.
The rotation of the clamp is evaluated using the rotation tensor. Since deformations are small, the components of the rotation tensor equal the angle given in radians. In Figure 5, the results are displayed in degrees. The rotation varies slightly over the generatrix of the inner sleeve surface. The computation gives an inclination value of approximately 0.5 degrees when both mounting bolts are present and tightened properly. This value is less than the maximum allowed angle of 1 degree. However, if one of the bolts is missing, the angle increases to approximately 1.75 degrees, which significantly exceeds the allowed inclination.
Figure 5: Rotation along the clamp.
Application Library path: COMSOL_Multiphysics/Structural_Mechanics/feeder_clamp
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Structural Mechanics>Solid Mechanics (solid).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click  Done.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
Ffeeder
2000[N]
2000 N
Feeder force
Afeeder
pi*20[mm]*20[mm]
0.0012566 m²
Feeder area
Fscrew
0.2*4500[N]
900 N
Screw force
D
7[mm]
0.007 m
Outer diameter
d
3.75[mm]
0.00375 m
Inner diameter
Awasher
pi/4*(D^2-d^2)
2.744E-5 m²
Washer area
W
20[mm]
0.02 m
Clamp width, z direction
To add a parameter, you can either edit directly in an empty table row or use the text fields below the table and click Move Up when you are finished (you might need to click on the table row to activate the text fields first).
Geometry 1
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose mm.
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, locate the Unite Objects section.
3
Clear the Unite objects check box.
4
Click  Show Work Plane.
Work Plane 1 (wp1)>Circle 1 (c1)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type 15.
4
Locate the Position section. In the xw text field, type 15.
5
In the yw text field, type 35.
6
Click  Build Selected.
Work Plane 1 (wp1)>Rectangle 1 (r1)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 20.
4
In the Height text field, type 55.
5
Locate the Position section. In the xw text field, type 5.
6
In the yw text field, type 5.
7
Click  Build Selected.
8
Click the  Zoom Extents button in the Graphics toolbar.
Difference 1 (dif 1)
Select both the circle and the rectangle (c1 and r1).
Work Plane 1 (wp1)>Difference 1 (dif1)
1
In the Work Plane toolbar, click  Booleans and Partitions and choose Difference.
2
In the Settings window for Difference, click  Build Selected.
Work Plane 1 (wp1)>Circle 2 (c2)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type 15.
4
Locate the Position section. In the xw text field, type 15.
5
In the yw text field, type 35.
6
Click  Build Selected.
Work Plane 1 (wp1)>Circle 3 (c3)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type 10.
4
Locate the Position section. In the xw text field, type 15.
5
In the yw text field, type 35.
6
Click  Build Selected.
Work Plane 1 (wp1)>Rectangle 2 (r2)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 1.5.
4
In the Height text field, type 20.
5
Locate the Position section. In the xw text field, type 14.25.
6
In the yw text field, type 40.
7
Click  Build Selected.
Work Plane 1 (wp1)>Compose 1 (co1)
1
In the Work Plane toolbar, click  Booleans and Partitions and choose Compose.
2
Click in the Graphics window and then press Ctrl+A to select all objects.
3
In the Settings window for Compose, locate the Compose section.
4
In the Set formula text field, type (dif1+c2)-(c3+r2).
5
Click  Build Selected.
Work Plane 1 (wp1)>Split 1 (spl1)
1
In the Work Plane toolbar, click  Conversions and choose Split.
2
Select the object co1 only.
3
In the Settings window for Split, click  Build Selected.
Work Plane 1 (wp1)>Rectangle 3 (r3)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 30.
4
In the Height text field, type 5.
5
Click  Build Selected.
6
Click the  Zoom Extents button in the Graphics toolbar.
Work Plane 1 (wp1)
1
In the Model Builder window, click Work Plane 1 (wp1).
2
In the Settings window for Work Plane, click  Build Selected.
Extrude 1 (ext1)
1
In the Geometry toolbar, click  Extrude.
2
Select the object wp1.r3 only.
3
In the Settings window for Extrude, locate the Distances section.
4
In the table, enter the following settings:
Distances (mm)
40
5
Click  Build Selected.
6
Click the  Go to Default View button in the Graphics toolbar.
Move 1 (mov1)
1
In the Geometry toolbar, click  Transforms and choose Move.
2
Select the object ext1 only.
3
In the Settings window for Move, locate the Displacement section.
4
In the z text field, type -10.
5
Click  Build Selected.
Extrude 2 (ext2)
1
In the Geometry toolbar, click  Extrude.
2
Select the objects wp1.spl1(1), wp1.spl1(2), and wp1.spl1(4) only.
3
In the Settings window for Extrude, locate the Distances section.
4
In the table, enter the following settings:
Distances (mm)
10
5
Click  Build Selected.
Move 2 (mov2)
1
In the Geometry toolbar, click  Transforms and choose Move.
2
Select the objects ext2(1), ext2(2), and ext2(3) only.
3
In the Settings window for Move, locate the Displacement section.
4
In the z text field, type 5.
5
Click  Build Selected.
Extrude 3 (ext3)
1
In the Geometry toolbar, click  Extrude.
2
In the Settings window for Extrude, locate the Distances section.
3
In the table, enter the following settings:
Distances (mm)
20
4
Click  Build Selected.
5
Click the  Go to Default View button in the Graphics toolbar.
Work Plane 2 (wp2)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, locate the Plane Definition section.
3
From the Plane list, choose yz-plane.
4
In the x-coordinate text field, type 5.
5
Locate the Unite Objects section. Clear the Unite objects check box.
6
Click  Show Work Plane.
Work Plane 2 (wp2)>Plane Geometry
1
In the Settings window for Plane Geometry, locate the Visualization section.
2
Find the In-plane visualization of 3D geometry subsection. Clear the Intersection (green) check box.
3
Clear the Coincident entities (blue) check box.
Work Plane 2 (wp2)>Circle 1 (c1)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Position section.
3
In the xw text field, type 55.
4
In the yw text field, type 10.
5
Locate the Size and Shape section. In the Radius text field, type 1.875.
6
Click  Build Selected.
Work Plane 2 (wp2)>Circle 2 (c2)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Position section.
3
In the xw text field, type 55.
4
In the yw text field, type 10.
5
Locate the Size and Shape section. In the Radius text field, type 3.5.
6
Click  Build Selected.
Difference 1 (dif 1)
Select both circles (c1 and c2).
Work Plane 2 (wp2)>Difference 1 (dif1)
In the Work Plane toolbar, click  Booleans and Partitions and choose Difference.
Work Plane 2 (wp2)>Circle 3 (c3)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Position section.
3
In the xw text field, type 55.
4
In the yw text field, type 10.
5
Locate the Size and Shape section. In the Radius text field, type 1.875.
6
Click  Build Selected.
Work Plane 2 (wp2)>Rectangle 1 (r1)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 5.
4
In the Height text field, type 10.
5
Locate the Position section. In the xw text field, type 55.
6
In the yw text field, type 5.
7
Click  Build Selected.
Work Plane 2 (wp2)>Circle 4 (c4)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Position section.
3
In the xw text field, type 55.
4
In the yw text field, type 10.
5
Locate the Size and Shape section. In the Radius text field, type 5.
6
Click  Build Selected.
Work Plane 2 (wp2)>Compose 1 (co1)
1
In the Work Plane toolbar, click  Booleans and Partitions and choose Compose.
2
Select the objects c3, c4, and r1 only.
3
In the Settings window for Compose, locate the Compose section.
4
In the Set formula text field, type r1-c4+c3.
5
Click  Build Selected.
Work Plane 2 (wp2)
1
In the Model Builder window, click Work Plane 2 (wp2).
2
In the Settings window for Work Plane, click  Build Selected.
3
Click the  Go to Default View button in the Graphics toolbar.
Extrude 4 (ext4)
1
In the Geometry toolbar, click  Extrude.
2
Select the object wp2.co1 only.
3
In the Settings window for Extrude, locate the Distances section.
4
In the table, enter the following settings:
Distances (mm)
9.25
5
Click  Build Selected.
Copy 1 (copy1)
1
In the Geometry toolbar, click  Transforms and choose Copy.
2
Select the object ext4 only.
3
In the Settings window for Copy, locate the Displacement section.
4
In the x text field, type 10.75.
5
Click  Build Selected.
Copy 2 (copy2)
1
In the Geometry toolbar, click  Transforms and choose Copy.
2
Select the object wp2.dif1 only.
3
In the Settings window for Copy, locate the Displacement section.
4
In the x text field, type 20.
5
Click  Build Selected.
Difference 1 (dif1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Difference.
2
Select the objects mov2(2) and mov2(3) only.
3
In the Settings window for Difference, locate the Difference section.
4
Find the Objects to subtract subsection. Select the  Activate Selection toggle button.
5
Select the objects copy1 and ext4 only.
6
Click  Build Selected.
7
Click the  Go to Default View button in the Graphics toolbar.
Work Plane 3 (wp3)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, locate the Plane Definition section.
3
From the Plane type list, choose Face parallel.
4
On the object mov1, select Boundary 2 only.
5
Click  Show Work Plane.
Work Plane 3 (wp3)>Rectangle 1 (r1)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Position section.
3
In the xw text field, type -5.5.
4
In the yw text field, type -15.
5
Locate the Size and Shape section. In the Width text field, type 11.
6
In the Height text field, type 5.
7
Click  Build Selected.
Work Plane 3 (wp3)>Circle 1 (c1)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type 2.5.
4
Locate the Position section. In the xw text field, type -5.5.
5
In the yw text field, type -12.5.
6
Click  Build Selected.
Work Plane 3 (wp3)>Circle 2 (c2)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Position section.
3
In the xw text field, type 5.5.
4
In the yw text field, type -12.5.
5
Locate the Size and Shape section. In the Radius text field, type 2.5.
6
Click  Build Selected.
Work Plane 3 (wp3)>Union 1 (uni1)
1
In the Work Plane toolbar, click  Booleans and Partitions and choose Union.
2
Click in the Graphics window and then press Ctrl+A to select all objects.
3
In the Settings window for Union, click  Build Selected.
Work Plane 3 (wp3)>Copy 1 (copy1)
1
In the Work Plane toolbar, click  Transforms and choose Copy.
2
Select the object uni1 only.
3
In the Settings window for Copy, locate the Displacement section.
4
In the yw text field, type 25.
Work Plane 3 (wp3)
1
In the Model Builder window, click Work Plane 3 (wp3).
2
In the Settings window for Work Plane, click  Build Selected.
3
Click the  Zoom Extents button in the Graphics toolbar.
Extrude 5 (ext5)
1
In the Geometry toolbar, click  Extrude.
2
In the Settings window for Extrude, locate the Distances section.
3
In the table, enter the following settings:
Distances (mm)
5
4
Select the Reverse direction check box.
5
Click  Build All Objects.
Difference 2 (dif2)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Difference.
2
Select the object mov1 only.
3
In the Settings window for Difference, locate the Difference section.
4
Find the Objects to subtract subsection. Select the  Activate Selection toggle button.
5
Select the object ext5 only.
6
Click  Build Selected.
Union 1 (uni1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Union.
2
Click in the Graphics window and then press Ctrl+A to select all objects.
3
In the Settings window for Union, click  Build Selected.
Rotate 1 (rot1)
1
In the Geometry toolbar, click  Transforms and choose Rotate.
Make sure the geometry is selected. If not, click on the geometry in the Graphics window to select it.
2
In the Settings window for Rotate, locate the Rotation section.
3
In the Angle text field, type 90.
4
From the Axis type list, choose Cartesian.
5
In the x text field, type 1.
6
In the z text field, type 0.
7
Click  Build All Objects.
Form Union (fin)
1
In the Model Builder window, click Form Union (fin).
2
In the Settings window for Form Union/Assembly, click  Build Selected.
3
Click the  Go to Default View button in the Graphics toolbar.
Add Material
1
In the Home toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in>Aluminum.
4
Click Add to Component in the window toolbar.
5
In the Home toolbar, click  Add Material to close the Add Material window.
Solid Mechanics (solid)
The boundary conditions consist of loads and constraints. The latter model the mounting bolts by setting the displacement to zero at the mounting holes off the clamp. All other boundaries are free.
Boundary Load 1
1
In the Model Builder window, under Component 1 (comp1) right-click Solid Mechanics (solid) and choose Boundary Load.
2
Select Boundary 22 only.
It might be easier to select the correct boundary by using the Selection List window. To open this window, in the Home toolbar click Windows and choose Selection List. (If you are running the cross-platform desktop, you find Windows in the main menu.)
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the FA vector as
Fscrew/Awasher
x
0
y
0
z
Boundary Load 2
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundary 68 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the FA vector as
-Fscrew/Awasher
x
0
y
0
z
Boundary Load 3
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundaries 11, 12, 43, and 47 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the FA vector as
0
x
Ffeeder/Afeeder
y
0
z
Fixed Constraint 1
1
In the Physics toolbar, click  Boundaries and choose Fixed Constraint.
2
Select Boundaries 34, 35, 38, 39, 62, and 63 only.
Assign the constraint grouping to be able to disable or enable the corresponding constraint in a parametric analysis.
3
In the Physics toolbar, click  Constraint Group and choose New Constraint Group.
Fixed Constraint 2
1
Right-click Fixed Constraint 1 and choose Duplicate.
2
Select Boundaries 32, 33, 36, 37, 60, and 61 only.
3
In the Physics toolbar, click  Constraint Group and choose New Constraint Group.
Mesh 1
Swept 1
In the Mesh toolbar, click  Swept.
Size
1
In the Model Builder window, click Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extremely fine.
Swept 1
1
In the Model Builder window, click Swept 1.
2
In the Settings window for Swept, click to expand the Source Faces section.
3
Select Boundaries 18 and 22 only.
4
Click  Build All.
Study 1
Step 1: Stationary
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, click to expand the Study Extensions section.
Set up two load cases, the first one with both mounting bolts present, and the second case, when one of the bolts is either significantly loosen or missing completely.
3
Select the Define load cases check box.
4
Click  Add.
5
Click  Add.
6
In the table, enter the following settings:
Load case
cg1
cg2
Load case 1
√
√
Load case 2
√
 
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node, then click Stationary Solver 1.
3
In the Settings window for Stationary Solver, click to expand the Output section.
4
Clear the Reaction forces check box.
5
In the Study toolbar, click  Compute.
Results
The default plot shows the stress distribution over the deformed geometry. Change it to visualize the displacement in the loading direction.
y-Displacement LC1
1
In the Model Builder window, under Results click Stress (solid).
2
In the Settings window for 3D Plot Group, type y-Displacement LC1 in the Label text field.
Surface 1
1
In the Model Builder window, expand the y-Displacement LC1 node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Solid Mechanics>Displacement>Displacement field - m>v - Displacement field, Y component.
3
In the y-Displacement LC1 toolbar, click  Plot.
4
Click the  Zoom Extents button in the Graphics toolbar.
The plot seems to indicate that the gap in the sleeve has been shut. However, this is an artifact of the default scale factor being larger than 1. To get an accurate view of the size of the deformation, set the scale factor to 1.
Deformation
1
In the Model Builder window, expand the Surface 1 node, then click Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor check box.
4
In the associated text field, type 1.
y-Displacement LC1
1
In the Model Builder window, click y-Displacement LC1.
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Load case list, choose Load case 1.
4
In the y-Displacement LC1 toolbar, click  Plot.
5
Click the  Zoom Extents button in the Graphics toolbar.
The resulting plot should be similar to that shown in Figure 2. Thus, there is still a narrow gap in the sleeve (if necessary, rotate the geometry in the Graphics window to get a better view).
y-Displacement LC2
Now, duplicate the plot to shown the second case with one of the mounting bolts missing, Figure 3.
1
Right-click y-Displacement LC1 and choose Duplicate.
2
In the Settings window for 3D Plot Group, type y-Displacement LC2 in the Label text field.
3
Locate the Data section. From the Load case list, choose Load case 2.
4
In the y-Displacement LC2 toolbar, click  Plot.
5
Click the  Zoom Extents button in the Graphics toolbar.
Proceed to reproduce the plot shown in Figure 4.
x-Displacement
1
In the Home toolbar, click  Add Plot Group and choose 3D Plot Group.
2
In the Settings window for 3D Plot Group, type x-Displacement in the Label text field.
Surface 1
1
Right-click x-Displacement and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type u*(abs(u)>0.25[mm]).
4
Locate the Coloring and Style section. From the Color table list, choose RainbowLight.
5
In the x-Displacement toolbar, click  Plot.
6
Click the  Zoom Extents button in the Graphics toolbar.
You can flip the Load case selector on the plot Data tab to see that the increase in inclination has almost no effect on the clamp deformation due to the screw forces.
Examine the resulting rotation of the clamp by evaluating the rotation of the deformation tensor.
Rotation
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Rotation in the Label text field.
Line Graph 1
1
Right-click Rotation and choose Line Graph.
2
Select Edge 95 only.
3
In the Settings window for Line Graph, click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Solid Mechanics>Strain>Rotation of deformation tensor>solid.RotyZ - Rotation of deformation tensor, yZ component.
4
Locate the y-Axis Data section. In the Expression text field, type solid.RotyZ*180/pi.
5
Click to expand the Legends section. Select the Show legends check box.
Rotation
1
In the Model Builder window, click Rotation.
2
In the Settings window for 1D Plot Group, locate the Plot Settings section.
3
Select the y-axis label check box.
4
In the associated text field, type Rotation of deformation tensor, yz component (deg).