A Catalog Feature is a predefined Sketch or Feature that can be inserted into a model with a single command. The sketch variation of the Catalog Feature allows inserting a sketch that is completely drawn, constrained and dimensioned.
Although equations can be used to define the sketch in the Catalog Feature, only the actual parameter values will be inserted with the sketch, and any formulas will be lost. This prevents creating a catalog feature whose dimensions will automatically adjust to existing parameters within a part. If you need the Catalog Feature to use a formula or part value, you must edit the Catalog Feature parameters after insertion and change the equations to formulas or part values.
In this tutorial we will cover taking a sketch of a Raised Panel cutter profile, and create a sketch Catalog Feature. That cutter profile can then be inserted into a part model, and be used to create a new feature based on the sketched profile. Another Instructable will use this sketch Catalog Feature to create a Raised Panel part with this profile defining the raised panel profile.
If you want to create a sketch Catalog Feature from an existing sketch that is already used to create a Feature, you must first delete that Feature to allow the creation of the Catalog Feature. Just make sure the part is saved that contains the desired sketch, delete the feature that uses the sketch, create the Catalog Feature, and then quit WITHOUT saving the changes to the part file.
Step 1: Create Sketch
The first step is to create a new Part, and draw the desired sketch. Fully constrain and dimension the sketch. You need to make sure that everything is fully constrained and dimensioned, as the Catalog Feature will be moved and re-oriented during insertion. If it is not fully constrained, the sketch may come apart while it is being manipulated. Orientation is not important as the Catalog Feature can be re-oriented and moved upon insertion if constructed properly.
Another important consideration is to avoid any undesirable implied constraints that would prevent the sketch from being relocated after insertion. Avoid use of the Origin or Reference Axes, and keep lines from being drawn on them. It is also a good idea to avoid moving the sketch about after being drawn to avoid any other implied locating constraints. We will address attempts to fix undesired constraints being inserted into the Catalog Feature at the end of this tutorial.
We prefer to create our Catalog Features in the upper right quadrant of the XY plane, and generally orient cutters similarly to their orientation in sales literature. In fact, we often insert a vendor graphic or scan of the cutter outline (traced onto paper) into an Alibre drawing, scale it to actual size, and do our best to trace the outline.
Below is a sketch of an example of a Raised Panel cutter profile. This profile was taken from an image downloaded from the vendors site on the Internet, and the values listed in the sales literature. The information is often less than complete, and this sketch should not be relied upon to be totally accurate and should be verified from the actual cutter.
Step 2: Mirror Cutter Profile
We have found that it is worthwhile to mirror cutter profiles, as the opposite hand orientation is often required to properly create a feature from the sketch. Take this into consideration when creating a sketch for a Catalog Feature, and possibly mirror your sketch.
When creating cutter profiles, it is handy to properly locate and define the axis of rotation so that it can be used to mirror the profile.
After creating the sketch, right click on the line about which the profile will be mirrored and select “Convert to Reference Figure” to convert the Regular figure to a Reference figure. A valid sketch has to be a SINGLE closed figure, and a Regular line dividing the two mirrored halves will prevent the successful creation of a Feature.
Step 3: Mirror the Sketch
Mirror the sketch by selecting the Mirror icon to open the Mirror Figure dialog; select the figures to mirror which are the sketch figures for the cutter profile; click in the Mirror axis: box of the Mirror Figure dialog window; and then select the just converted Reference Line for the mirror axis. When the preview correctly shows the mirrored figure, select the OK button on the Mirror Figure dialog to create the mirrored figures.
There will be a number of symmetric constraint icons inserted as they constrain the new figures to the original figures symmetrically about the mirror axis.
It would be prudent to save the part file at this point. Since there is no feature created from this sketch, it will appear to be empty except for the sketch listed in the Design Explorer. You can save the part file under the same name you wish to use for the Catalog Feature as they have different filename suffixes. The Catalog Feature suffix is .AD_PCF, and will be the only files displayed in the dialog to insert a catalog feature.
Step 4: Rename the Sketch & Parameters
The name of the Sketch listed in the Design Explorer will determine the name listed when the Catalog Feature is inserted into a Part. The name of the Part used to create the Catalog Feature will not have any bearing on the description of the new catalog feature sketch inserted into the destination Parts Design Explorer.
Rename the sketch to an apt description for the Catalog Feature sketch. Once inserted into the destination part, the sketch will be have “_Catalog Feature” automatically appended to the sketch name. You can then rename the sketch in the destination part if desired.
Additionally, all the parameters defined for this sketch will be included in the destination parts Equation Editor. The parameter name will have an sequenced identifier appended to the end upon insertion of the Catalog Feature. Each insertion of the Catalog Feature sketch will have a unique set of sequenced identifiers appended to the end of the parameter name. You can then rename the parameters in the destination part, bearing in mind that you can not have two parameters with the same name. Often it is best to provide a descriptive name for the parameters used in the Catalog Feature that will not only identify the origin of the parameters, but help in determining the proper parameter for possible modification.
Since only a parameter value will be inserted with the Catalog Feature, it is often the case that these parameters’ Equations will have to be modified to include part value parameters or formulas. For example, a cutters profile depth may be changed to and equation of “Thick” or a fraction thereof. It is worth spending some time now to properly identify the parameters.
Step 5: Create the Sketch Catalog Feature
Make sure that a sketch is not currently being edited, and from the top menu select FEATURE > SAVE CATALOG FEATURE ...
You can then select the desired sketch for the Catalog Feature, or if selected before the save, the sketch will automatically populate the Save Catalog Feature dialog box.
If the sketch needs to be replaced in the Save Catalog Feature dialog box, just select the Exported Feature box, and then the appropriate sketch.
Select the Save As... button and the save dialog box will appear. Make sure the proper location and name for the Catalog Feature is selected, and then Save.
We have created a Catalog Feature folder in which we store most of our standard Catalog Features.
You have now created a Catalog Feature of a Sketch.
Step 6: Troubleshooting Catalog Features
A Catalog Feature file can be opened similar to a part file, in order to fix any problems. The main difference being that a Base Feature is now included in addition to the sketch for the Catalog Feature.
The Catalog Feature sketch can be edited as with any other sketch and any required corrections or changes can be made. While the Catalog Feature file can be modified and updated, it is still prudent to save the original part file used to create the Catalog Feature. If necessary, the Base Feature can be deleted and a Save As.. used to create a new part file to create subsequent Catalog Feature(s).
The most common problem encountered with a Catalog Feature is the inclusion of Fixed Constraint due to some implied constraint inadvertently created with the sketch. This will prevent the Catalog Feature sketch from being relocated and constrained in the desired position. With the Select Cross active, simply hover over the offending constraint, right click, and select Delete from the pop up menu.
Another common problem is the lack of complete constraints for the sketch and the Catalog Feature comes apart while being manipulated. Instead of going back to the original Part, and attempt can be made to correct the problem and provide additional constraints directly to the sketch in the Catalog Feature. If successful, remember to make the same corrections to the original part file.
Remember, a Catalog Feature sketch has to be fully constrained and dimensioned or it will come apart or have figures change size while being manipulated.