Sheet Metal Punch iFeatures - part 1
Estimated Time Required to Complete: 45 minutes
|This is part 1 of a skill building exercise exploring sheet metal punch iFeatures. It covers creating sheet metal punch iFeatures. |
In This Exercise
In this skill building exercise you will explore the creation of a simple Sheet Metal Punch iFeature. After you have completed this exercise you should understand:
- The steps required to create a family of simple Sheet Metal Punch iFeatures which can be used to cut material from sheet metal parts of different material thicknesses.
- The similarities (and differences) between Sheet Metal Punch iFeatures and “regular” iFeatures.
To complete this exercise you will:
- Download and open a zip file containing a sheet metal part.
- Extract the cut feature from the source part and save it as a Sheet Metal Punch iFeature capable of making cuts of several sizes in other sheet metal parts of various thicknesses.
|Note – all images shown in this document were created using the Inventor color scheme named: Presentation. The colors you see may not agree with the included images depending on the scheme you have selected. |
Prior to working this exercise you should:
- Have Inventor R2008 installed.
- Understand how to open, create and save part and sheet metal part files in your active project. If you have not completed the Building Sheet Metal Parts tutorial supplied with Inventor you should do that before working this skill builder (from the Inventor Help menu select Tutorials, then select Building Sheet Metal Parts from the Basics portion of the tutorials launch pad).
- Understand sheet metal part styles including material and thickness.
- Download (and unzip) the zip file containing the source file that will be used during this exercise.
The zip file contains an Autodesk Inventor R2008 sheet metal part file:
The part contains the cut feature which will be used to create the Sheet Metal Punch iFeature.
Sheet Metal Punch iFeature Overview
Sheet Metal Punch iFeatures are named collections of Autodesk Inventor features that can be placed in sheet metal part models to represent the result of a punching operation.
Sheet Metal Punch iFeatures are not models of the physical punch (and die) used to create a particular end result on a sheet metal piece part. To create a Sheet Metal Punch iFeature you will not model the punch and die tooling shown in the above illustration.
While it is possible to create a Sheet Metal Punch iFeature that represents a single size feature it is much more likely that you will define a family of punches that create various sized features which are identified by a “key” dimensional value. While Autodesk Inventor supports the creation of iFeatures which accept any value to drive the size of the resulting feature, Sheet Metal Punch iFeatures usually represent physical tooling and are frequently created using a limited set of listed values that represent stock tooling sizes.
Creating a sketch that behaves predictably requires fully constrained geometry with dimensions, dimensions driven by parameters and geometric constraints.
The sketches used to define Sheet Metal Punch iFeatures must also contain a center point. The sketch center point is used to define the position of the punch during placement within the part model. It will automatically position the punch over corresponding unconsumed center points on visible sketches within the sheet metal part.
This center point requirement is one way that a Sheet Metal Punch iFeature differs from a “regular” iFeature. In addition to all of the information that is required by a “regular” iFeature, Sheet Metal Punch iFeatures can also contain:
- A site-specific Punch ID designation that can be used on your drawings to identify specific tooling in your shop’s tool inventory.
- A simplified sketch that can be used to represent the punch on drawings in the event that the complete geometric representation would unnecessarily complicate the drawing.
- A custom depth designation that would be used primarily during the drawing annotation of formed punch features of coined or stamped features.
The fields for these additional parameters are enabled on the Extract iFeature dialog when the Sheet Metal Punch iFeature radio button is selected.
|Creating a Sheet Metal Punch iFeature which uses this additional data will be covered in a separate skill building exercise. |
Open and Examine the Supplied Source File
1. Open the punch01_source.ipt file included in the downloaded zip file. The part contains a cut feature on the single face. As can be seen, there is a sketch located under the cut feature.
2. Right mouse-click Sketch2 and select Visibility from the context menu to turn the visibility of the sketch on. Notice that the sketch consists of two trimmed circular arcs, dimensions on these arcs and a center point that has been located at the center of the larger circular arc.
3. After you have examined the sketch, toggle the visibility off (right mouse-click Sketch2 and select Visibility again).
Extract the Sheet Metal Punch iFeature
1. Select Extract iFeature… from the Tools menu to open the Extract iFeatures dialog.
|Each time the Extract iFeature dialog is opened an iFeature icon is displayed at the top of the Selected Features browser (in the dialog) followed by a temporary name for the new iFeature. The temporary name is sequentially numbered. Your temporary name will likely differ from the name shown in the illustrations. |
2. Select the Sheet Metal Punch iFeature radio button option at the top of the Extract iFeatures dialog.
3. In the part browser, click on Cut1 to identify the feature that you want to extract. Notice that following your selection in the part browser, information populates the Extract iFeature dialog.
4. In the Selected Features area of the dialog, select the line that reads:
x= d3 (0.3750000 in)
This parameter defines the radius of the large circular arc.
The line will highlight and the >> button will enable. You want to move this parameter into the Size Parameters area, to do so select the >> button. The parameter is now included in the Size Parameters area.
5. You want to define a list of selectable values that can be used to drive the size of the punch you are creating - in the Size Parameters area of the dialog, select the value None in the Limit column of the d3 parameter row.
6. Select the displayed dropdown arrow.
7. From the list of option selections select: List.
8. In the List Values dialog that opens, click on the line that reads:
Click here to add value
Enter a value of: 0.5 in
Repeat the process and enter a value of: 0.25 in
You now have three selectable values which will define valid radii for the punched feature: 0.25”, 0.375” and 0.5”. The List Values dialog also provides you with the ability to define which of these values will be selected by default when you place the punched feature. In this exercise we will leave the value at 0.375”
Click OK to accept the two values you added and to dismiss the List Values dialog.
9. You should now modify the prompt text that will be displayed when you select this value during placement – select the text string that reads:
Change this string to read:
10. Next you must identify the positioning geometry which in the case of a Sheet Metal Punch iFeature is the sketch containing the center point (in this example: Sketch2 located under Cut1 in the part feature browser). Click to the left of the name text: Profile Plane1 in the Position Geometry portion of the Extract iFeature dialog.
In the above illustration, the sketch grid lines are displayed in the graphics window following this selection. Note – these lines will only be visible if the application option to display the sketch grid lines and minor grid lines is enabled (if you have not modified the defaults, this option should be enabled).
11. In the part browser, select Sketch2 (the sketch containing the positioning center point for this punch).
Save the Sheet Metal Punch iFeature
While it would be possible to define more options for this punch (for example: the radius of the location notch could be included as a size parameter and assigned a list of acceptable values) for this exercise we will consider our punch defined and save what we have.
1. On the Extract iFeature dialog select the Save button.
2. The Save As dialog will display.
Assuming that you (or your system administrator) have not modified the defaults found in Tools|Application Options for iFeatures the Save As dialog should open with the supplied Catalog folder as the active folder.
3. You will want to save your punch with other punches, so in the Save As
dialog double-click on the folder named Punches
and type in a meaningful file name. For this exercise use the following:
notched hole .25 .375 .5
4. Click the Save button and then click Yes on the dialog that warns you that the location is not within your active project.
|Note – there are a number of ways to avoid seeing the above dialog including: using Autodesk Vault, adding the location specified in Application Options to your specific project(s) or simply selecting the Prompts option and opting not to see the dialog. Saving your Sheet Metal Punch iFeature *.ide files outside of the active project has no impact on the integrity of the file or your ability to subsequently use the punch defined. |
Congratulations! You have just created and saved your first sheet metal punch iFeature.
Let’s review your accomplishments…
In this introductory skill building exercise you:
- Used a supplied part with a single cut feature to create a single sheet metal punch iFeature file that contained three punch definitions – each a specific size.
- Reviewed the sketch in the supplied part to understand the importance of dimensions, constraints and parameters in the creation of well-behaved sheet metal punch iFeatures.
- Reviewed the differences between sheet metal punch iFeatures and “regular” iFeatures. These include:
- The need for a center point in the defining sketch for sheet metal punch iFeatures
- Use of the sheet metal punch radio button option on the Extract iFeature dialog
- Optional use of: Punch ID, alternative representations and custom depth (covered in depth in a separate skill building exercise)
- Learned the location of the Extract iFeature tool (under the Tools main menu).
- Learned how to select features in the source model that will become re-useable iFeatures
- Learned how to select parameters which drive selected features and to use those parameters to define iFeature variations that define a punch iFeature of a specific size.
- Learned to modify prompts that will appear during punch placement.
- Learned to select the sketch containing the defining center point of your punch feature which will position your punch during placement.
- Learned to save your punch iFeature in the default location (with brief mention of other data management possibilities).
In the next skill building exercise in this series you will place the punch you just created on a supplied target part. Close the currently open punch01_source.ipt file.
This exercise only scratches the surface – to continue building your sheet metal punch skills you should work through the next skill builder in this series in which you will place the punch you created in this exercise on a sheet metal part. You could also:
- Create your own (more complex) sheet metal cut feature and extract that to create a more complex punch family.
- Work through the Creating iFeatures tutorial installed with Inventor 2008. Select Tutorials from the main Help menu and then select the Creating iFeatures tutorial from the Advanced area of the tutorial selections.