SolidWorks Tutorial(几何提取)

SolidWorks Tutorial: External Gear Pump

Aaron Heisler

University of Wisconsin

Powertrain Control Research Laboratory

May 23, 2008

Goal: The purpose of this document is to assist PumpLinx users in transferring a CAD file of an external gear pump modeled in SolidWorks to the required STL file format for PumpLinx.

1.To begin, a complete pump model must be created. An example of such a model is

shown in Figures 1 and 2. At this stage, the model must have all the geometric features the user wishes to be included in the PumpLinx analysis.

Figure 1: To begin, the pump model must be complete in every detail

required for the analysis.

Figure 2: The gear timing is important at this stage in the analysis.

There are a few areas which need special attention so the simulation can be properly set-up. These issues include the following:

?The side face of the gear must have zero gap between it and the bushing.

?The gaps between the teeth must be large enough that the gears do not cross at any point during a revolution of the input shaft. For the pump shown in Figures 1

and 2, the minimum gap was approximately 0.0034 in. The magnitude of the gap

will depend upon the individual pump design.

?The exact center location of the gears must be known. For simplification later on, mate the assembly origin to the center of one of the bottom gears and add parallel

mates between the assembly planes and part planes. The purpose of this step is to

ensure that the pump is aligned to a specific coordinate system that can be easily

referenced at any point in time.

2.Now that the pump geometry is finished to the level of detail desired for the analysis, the

fluid region must be extracted. This is done in two distinct steps. The first step extracts the fluid encompassed by the approximate “figure 8” volume the gears p ass through during one revolution of the input shaft. To extract this volume, execute the following steps:

a.Open a new part.

b.Draw a circle in any reference plane. Dimension the circle so it exactly matches

the diameter of the housing where the gear is located (see Figure 3).

c.Draw a circle of equal diameter to create a “figure 8” shaped sketch that fills the

void inside the housing shown in Figure 3. The final sketch should look similar to that shown in Figure 4.

Figure 3: The new part must have the same diameter as the holes bored

in the housing enclosing the gears.

Figure 4: The “figure 8” shaped part begins as a drawing containing two

equal diameter circles with a known center distance.

d.Extrude this shape to the exact width of the gears. The final part should be

similar to the volume shown in Figure 5.

Figure 5: Extrude the sketch to the exact width of the gears.

e.This part is then inserted into the pump assembly and mated such that it fills the

aforementioned void encasing the gears. The gear outline will still be visible since both parts are the exact same thickness.

Figure 6: The new part is inserted into the assembly and mated such

that it encapsulates the pair of gears and fills the housing bore.

f.Select the new part, and click “Edit Component” in the main toolbar. Then go to

“Insert” –“Mold” –“Cavity” as shown in Figure 7. For “Design Components”

select the two gears that this part encapsulates from the tree then click OK. Keep “Component Origins”, “Uniform Scaling”, and “0.00%” for the options.

Figure 7: To extract the fluid region around the gears, the “Cavity” feature will be used. Special care must be taken to ensure the proper region is extracted.

Figure 8: Select the two gears which the part is in plane with under “Design Components” and ensure no scaling is applied.

g. A new window will open titled “Bodies to Keep”. Click the “Selected bodies”

button and select the body that is the new part minus the gear volume. The small volumes at the center of the gears in Figure 9 should not be saved as those regions do not contain fluid in the actual pump.

Figure 9: Multiple volumes are created when the “Cavity” function is used. Pick the

appropriate body which equates to the volume of fluid trapped around the gears.

h.This part is now finished. Repeat this process for each pair of gears present in the

pump.

Figure 10: The finished part is the original “figure 8” shape with the

gear volume subtracted. This is the first of the two fluid regions

required and needs to be done for each pair of gears.

3.The second fluid volume can now be extracted from the gear pump assembly. Execute

the following steps:

a.Open a new part.

b.Create an arbitrary shape that fills the entire volume of the pump. The shape of

this part is not important and can be of nearly any design. The only important

note is that this part should have the same width as the distance between the inlet

and outlet port faces. Mate the inlet and outlet faces so they are coincident as

shown in Figure 12.

Figure 11: To extract the fluid trapped in the inlet and outlet ports,

create a large part that captures all the regions inside the pump that may

contain fluid which must be analyzed.

Figure 12: The new part is mated to the inlet and outlet ports and is

large enough to include any internal volumes that could contain fluid

inside the pump housing.

c.The same process as was used for the “figure 8” part will be used again to subtract

the pump volume from the new part. Select the new part from the tree and click “Edit Component”. Click “Insert” –“Mold” –“Cavity”. Pay special attention to the parts selected under “Design Components”. Select each housing section as

well as the “figure 8” parts created in Step 2 and the gears. Again, select

Component Origins from “Scale about”, “Uniform scaling: 0.00%”. Click OK.

Figure 13: When using the “Cavity” function to find the internal volumes of the pump,

be sure that all the parts including the pump housing, “figure 8” parts, and gears are

selected under “Design Components”.

d.When the “Bodies to Keep” window pops up, click the “Selected Bodies” button

and select the bodies that are the fluid volume from the inlet and outlet faces to the gears. Typically, “Body 1” and “Body 2” are the required volumes although this is dependent upon the internal pump design. Click OK.

e.The final part should look similar to the volume shown in Figure 14.

Figure 14: The final part should look similar to this.

4.The final step is to save the new parts in the correct format (.stl file extension). To do

this from the assembly, click “File” –“Save As”. Under “Save as type” click the drop down menu and select “STL”.

Figure 15: Select STL from the “Save as type” format. This is the file format PumpLinx

requires when importing a three-dimensional surface.

Click the “Options…” button at the bottom of the window. At this point, select the resolution that is appropriate for the application. For a finer mesh, select an Angle Tolerance of 1.0° and the minimum Deviation Tolerance. Click the check box in front of “Do not translate STL output data to positive space”! Neglecting this step will move the relative position of the parts when they are imported into PumpLinx. Then click “OK” and “Save”.

Figure 16: In the options menu, be sure to click the button “Do not translate STL output

data to positive space”. If this box is not checked, the origins of the part will be relocated

randomly when the parts are imported to PumpLinx.

Depending on the pump’s design, more than a dozen STL files will be created. Only the fluid region files are necessary for the PumpLinx analysis. In this example, the required files are the two “figure 8” shaped parts as well as the inlet and outlet port parts.