CREATING COPING PATTERNS IN AUTODESK INVENTOR



CREATING COPING PATTERNS IN AUTODESK INVENTOR

USING FRAME GENERATOR & SHEET METAL MODULES

These instructions will assist in creating coping patterns for fabrication using Inventor, without the need for manually modeling the individual frame members. Inventor’s Frame Generator will be used to create a representative model of the frame, then a series of sheet metal operations will be used to unfold the part into a coping pattern.

Frame Generator operates using the concept of Skeletal Modeling, a technique in which a reference part is used to define the locations and sizes of the actual components. The actual cross sections of the individual standard-sized frame members are then pulled from Content Center libraries, eliminating the need to model them individually.

Begin by creating a new assembly and saving it in the desired location.

Beginning in Inventor 2010, a new command was introduced to create this reference part for you. With the assembly still open, click the “Make Layout” button on the Assemble tab. Name this component appropriately, such as “Layout-Project Name.” It is good practice to leave the word “Layout” at the beginning of the name, as it makes it easier to find this part in the assembly later, should the parts ever be reordered in the browser. Verify that the template and new file location are correct, and then click OK.

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Figure 1: Make Layout Command

Depending on Application Options settings, you should now be editing a sketch within the new Layout part. This part will usually contain no solid geometry, and is used for reference when defining the frame. Draw the geometry required to define the frame (typically, for a coping pattern this will be a diagram representing the frame member centerlines). If building the frame manually rather than using the Frame Generator, it may also be helpful to add reference planes or points in the Layout part to aid in building the rest of the model.

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Figure 2 Sample Skeleton Sketch (Resulting Frame Shown in Gray)

Due to the limitations of the Frame Generator when dealing with round frame members, it is necessary to be especially careful when defining the skeleton sketch for frames that contain them. Frame Generator will create frame members that are the same length and location as the lines they reference in the sketch. If the vertical or diagonal sketch lines protruded down to the origin, crossing the horizontal line, the generated frame members would be too long, and would be difficult to trim.

Due to the Trim to Face command, this is not a problem with square or rectangular members. However, since this command does not work on round frame members, it is necessary to carefully consider locations where centerlines cross in round-member frames.

Once the skeleton sketch is complete, click Finish Sketch, then Return to the assembly. Click the Insert Frame Member button to begin placing members. This will bring up the Insert dialog box.

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Figure 3 Insert Frame Member Dialog Box

First, select the lines from the skeleton sketch which represent the member centerlines. Select the appropriate Standard, Type, and Size of frame members. If a required size is not available from the Content Center library, select the closest size and manually edit the dimensions later. When finished, click OK.

Note: If there are multiple sizes in your frame, you will need to start the command over for each size. It is possible to place multiple frame members at once, but they must be of the same size.

You should now have a crude representation of the frame. However, as can be seen with hidden lines turned on, the members are protruding into one another. It is now necessary to cut these members to match what is actually to be fabricated.

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Figure 4 Initial Frame Members

In this case, members B and C are meeting in a “T” shape, with member A coped to match up to both B and C. Were these frame members rectangular or square, the Trim To Face command could be used to clean up the intersections. However, this command does not work for round cross sections, and we must instead use several iterations of the Notch command.

First, we create a notch in member B, where it meets C. Click the Notch command; you will see the following dialog box.

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Figure 5 Notch Command Dialog Box

The frame members to be selected are color-coded. The blue member is the member to be cut – in the example, this would be member B. The yellow member is the mating part to fit in the notch – in this case, member C.

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Figure 6 Notched End of Member B

Member A must be notched to fit against both B and C. Two separate Notch commands must be used. Both will use A as the blue member, B and C will be used as the yellow members.

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Figure 7 Double-Notched End of Member A

The frame members now match up much as they would in the real fabricated frame. It is now possible to use the models to generate unfolded coping patterns to assist the fabricator in cutting the ends of the members.

Although these parts are not sheet metal, it is possible to use Inventor’s sheet metal commands to unfold the profile to make the coping pattern. To avoid disturbing relationships in the assembly, it is best if this is performed on a copy of the part model, rather than the original one created by Frame Generator.

It is possible to do this by manually copying and renaming the file. However, the ideal method is to use a Derived Component. A manual copy will not update if the original frame model changes – the Derived Component will allow the copy to update should the member size or frame geometry change later.

To create the derived copy, first determine the file name of the frame member to be coped, and then perform the following procedure.

1. Start a new part file. This should be created separately, not inside the frame assembly.

2. If a sketch is created upon part creation, click Finish Sketch, then delete it from the browser. No sketch is required for a derived component.

3. Save the part with an appropriate name, such as “Coping Pattern A.”

4. Click the Derived Component command, browse to the part file for the frame member to be coped, then click Open.

5. For this task, the default Derived Component setting of only deriving the solid body is acceptable, so click OK.

You will now have a part on your screen that looks identical to your frame member, except that its browser history begins with a copy of the original part. If the frame member is changed later, the derived copy will update accordingly.

To unfold the part into a flat pattern, it must first be converted to a sheet metal part so that the relevant commands will become available. Click Convert-Sheet Metal.

It is now necessary to set the sheet metal Thickness parameter to the wall thickness of the tube. Click Sheet Metal Defaults, then enter the member’s wall thickness in the Thickness box. If there is a parameter in the model controlling wall thickness, it is also possible to link this value to the parameter, so that they update together.

While editing the Sheet Metal Defaults, also change the Kfactor to .99. While this is not a realistic number for a steel part formed from sheet metal, setting this factor as close as possible to 1 eliminates corrections for stretching that we do not want included in our pattern.

Next we will use the Rip command to create a gap in the model that will allow it to unfold.

First, create a sketch on the flat end of the frame member. Draw a line between the projected circular edges. The line should be drawn such that, when projected along the length of the frame member, it will pass through one of the concave, coped sections (see red arrow).

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Figure 8 Rip Line Sketch

Start the Rip command. Set the gap size to .001 (this minimizes the amount of material removed by the gap left by the Rip command).

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Figure 9 Rip Dialog Box

Select the inner or outer surface of the cylinder as the Rip Face. The surface should be determined by looking at which one terminates last when travelling axially along the part. In this case, since the notch cut causes the inner surface to protrude beyond the outer, choose the inside surface. Selecting the incorrect surface may sometimes cause the Rip to terminate without cutting through the entire part, which will cause problems when unfolding the pattern.

Select the endpoint of the sketch line which intersects the Rip Face surface as the Sketch Point. Most of the time, it will be the only point that will allow picking.

There should now be a very small gap ripped along the part. Verify that the gap travels the entire length of the part before proceeding.

In some cases where an entire frame is being modeled, both ends of the part may be coped, and there will be no flat surface to sketch on for the Rip command. In these cases, it will usually be necessary to cut the gap manually with an Extrude command, using a profile .001” wide.

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Figure 10 Ripped Version of Part

Once the part has been successfully ripped, the Flat Pattern command may be used to unfold it. Click the command, which is located on the Sheet Metal tab, and the part will automatically be flattened.

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Figure 11 Unfolded Part

Using the Measure Distance tool, verify that the width of the unfolded part is acceptably close to the circumference of the original cylinder. Circumference may be found by calculation (π x D), or by measuring on the original model using Measure Loop.

If the unfolded part width is acceptable, you are ready to create the drawing that will be used to print the pattern for fabrication. Start a new drawing, then delete the title block and border from the browser. You should be left with a completely blank drawing sheet.

Place a base view of the flattened part. Select the appropriate view orientation, and set the scale to 1:1.

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Figure 12 Base View Dialog Box

Click to place the view. If necessary, resize the drawing sheet by right-clicking Sheet:1 in the Browser and clicking Edit Sheet in the menu. The view can also be rotated on the sheet by right-clicking it and selecting Rotate.

Once the view is positioned such that the coped end fits on the sheet at full scale, the drawing can be plotted and used for a pattern when coping the part.

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Figure 13 Finished Coping Pattern

If both ends are coped, depending upon the sizes involved it may be possible to use the Break command on the Place Views tab to crop out the middle of the pattern and show both ends on a single sheet of paper.

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Figure 14: View Break Used to Fit Pattern to Single Page

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