Improving Productivity with Parameters

Transcription

1 Improving Productivity with Parameters Michael Trull Rocky Brown Thursday, January 25, 2007

2 Improving Productivity with Parameters Part I The Fundamentals Parameters are variables which define the size and shape of part features and control the relative position of components within an assembly. In their simplest form, parameters are the dimensions we enter to define our models. But they can be so much more. Parameters can include equations defining functional relationships between them. A parameter s equation can include references to other parameters in the same sketch, in the same part, in other parts, or even in spreadsheets. Parameters can also be used in drawings. With so many options, parameters are a very powerful tool providing endless opportunities for increased productivity. This article gives users access to the power of parameters by showing how they are created and used in Autodesk Inventor. The article is broken into five installments covering: Part 1 The first installment introduces parameters by showing how they are created and the wealth of tools available for editing and maintaining them once they have been created. Part 2 The second installment builds on this introduction by showing how simple dimensions can be replaced with equations which help designers capture functional relationships and design intent. Part 3 The third installment expands the reach of parameters by showing how they can be exported and accessed by other parts. Part 4 The fourth installment shows how parts and assemblies can access a common set of parameters stored in an Excel spreadsheet. Part 5 The fifth and final installment winds up the series by showing how exported parameters can be accessed in drawings. How are parameters created? Parameters are created automatically when you define a sketch dimension, create a feature, or add an assembly constraint. When a parameter is created, inventor automatically assigns a parameter name, such as d0. As each parameter is created, Inventor assigns the next parameter in numerical sequence, such as d1, d2, and so forth. When a parameter is created, it is also assigned a numerical value, and a unit of measure. Each time you add a dimension or feature to the model, parameters are assigned. User parameters can used to define functional requirements. Both types can establish the relationships between the elements of a model. What is the Parameter Table? Parameters can be viewed or edited with the parameter tool. This brings up the parameter table, displaying names and values of the parameters automatically created during the modeling process. Clicking Update will apply any changes to a parameter, and any dependent parameter.

3 Figure 1: Parameter Table What is contained in the parameter table? Parameter Name is the name of the parameter. The default name of a parameter can be changed to a more descriptive name. Click in the box and enter the new name. When you update the model, all dependent parameters update to reflect the new name. Units are the units of measurement for the parameter. Equation generates the value of the parameter. If the parameter is a discrete value, the value is displayed exactly as it is entered. To change the equation, click the existing equation and enter the new equation. Nominal Value is the ideal value of the equation (displayed in full precision). Tolerance shows the current evaluated size setting for the parameter. Click a cell to select Upper, Nominal, or Lower settings. Model Value shows the actual calculated size of the parameter. Export parameters check box adds the parameter to the custom properties for the model. Custom properties can be added to parts lists and bills of materials. Selecting the check box will add the parameter to custom properties. Clearing the check box will remove the parameter from custom properties. Comment, if any, allows you to describe anything about the parameter. To add a comment, click in the box and enter the comment. What are User Parameters? User parameters are equations created by the user, and assigned to a unique parameter name. These parameters are used in equations to help define other parameters. Figure 2: User Parameters in the Parametric Table

4 How do I use parameters? For example, most dimensions in a part model are associative. The value can be edited and replaced by another value, or even an equation, such as (d0+3)*12. Notice what happens when you enter the equation. The equation now becomes (d0+3 in)*12 ul. Inventor automatically assumes the unit of measure in the equation. When an equation is entered in, the equation will remain black, indicating that it is logical and has the correct syntax. The equation will turn red if the equation cannot be calculated and the syntax is incorrect. Figure 3: Parameter Showing Correct - Incorrect Equations When an equation is added to a dimension parameter, the calculated dimension will show a prefix fx: in front of the dimensional value. Figure 4: Calculated Dimension Are there any rules for creating parameters? Follow these guidelines to make sure parameters and parts update predictably: Assign meaningful names to parameters. Equations cannot be recursive.

5 Parameter names cannot include spaces, mathematical symbols, or special characters. They are also case sensitive. If you link a spreadsheet to the parameters, you cannot edit its values or equations inside Autodesk Inventor (but must open and edit the spreadsheet in Microsoft Excel). How do I edit parameters? Parameters can be edited in several ways. The most common way is to use the parameter table. Parameter names, units, and equations may be edited. The value of a parameter can also be changed, by editing the sketch dimension or the feature. Dimension Properties can also be edited. Here s how. With any dimension visible, highlight the dimension, right click and select Dimension Properties. Figure 5: Selecting Dimension Properties

6 The Dimension Properties dialog is displayed. On the Dimension Settings tab, you can rename the parameter, and change the precision of the dimension. Tolerance settings can also be accessed. Figure 6: Dimension Properties Dialog By using this work flow, the parameter name can be changed in place, while viewing the dimension. When you combine using the Dimension Properties with the Edit Dimension dialog box, you do not have to go back and forth between the Parameter Table and the model. To edit the dimension value, just select a dimension and double-click it. You can make changes in the Edit Dimension Dialog box. Figure 7: Edit Dimension Dialog Box

7 If there are no dimensions visible, you can select a feature in the browser, right click and select Show Dimensions. Then, select the dimension value to be changed. Figure 8: Selecting Show Dimensions in the Browser

8 Improving Productivity with Parameters Part II Linking to Excel Spreadsheets Linking Parameters Externally There are two work flows to link parameters into a part or an assembly model: Excel spreadsheets and derived part files. Excel Spreadsheets Linking worksheets is the ability to control multiple part and assembly model files from one, master document. Excel has powerful calculation and logic functions, that allow the creator to make a user interface that is both easy to use. It also allows the most output with the least amount of user input. Advantages: Can be used to control many files at once Complex and logic calculations are performed in the Excel spreadsheet Can be used to validate or limit user input Disadvantages: Project sensitive. The Spreadsheet must remain in one of the specific project paths (but not a library path). It cannot be deleted like an embedded sheet. Changes to one file my conflict with another file within the assembly Some versions of Inventor have problems communicating with Excel without problems The process of linking an excel worksheet is easy. The creator has the option to create the part model first, create the Excel spreadsheet, Link it to the part model, and then edit the desired part parameters. The creator can also create the Excel spreadsheet first, create the part model, linking the Excel spreadsheet before creating any geometry, and use the parameter names as entries in dimension fields, or feature fields. Comparing an Excel Spreadsheet to a Parameter Table When setting up the Excel Spreadsheet, set it up similar to the Parameter Table. The spreadsheet should contain the same columns as the Parameter Table, with one exception. The units and equations columns must be flipped in the Excel spreadsheet. Since a starting cell will be defined when linking the spreadsheet, it is helpful to add the column headers across the top row, to avoid any confusion.

9 Figure 9: Parameters in the Excel Spreadsheet Another thing to remember is the way equations are defined. In Excel spreadsheets, the equation definition and calculations should be done in Excel, where the value is only exported to the model. Figure 10: Calculating Equations in Excel Spreadsheet

10 Improving Productivity with Parameters Part III Linking to Part and Assembly Models Linking to Existing Part and Assembly Models This assumes that the part and assembly files have been created, and that the Excel spreadsheet has been created. 1. Open the model file to which the Excel file will be linked. 2. Open the parameters dialogue and click Link. 3. In the open dialogue select the Excel file, select Link and enter the starting cell for the parameters. 4. Edit each feature and assign the parameter name to the value of the feature or sketch dimensions. Edit each feature or sketch dimension by their edit function or by the parameter table.

11 5. Repeat this process for each of the files in the assembly that require to be linked. 6. Make sure that if the part is used in an assembly, link the Excel spreadsheet to the assembly. Remember to be aware of the fact that linked Excel sheets are project specific. The Spreadsheet must remain in one of the specific project paths (but not a library path). It cannot be deleted like an embedded sheet. Linking to New Part and Assembly Models This assumes that the Excel spreadsheet has been created. 1. Create a new model file from a template, to which the Excel file will be linked. If you have the Sketch on New Part Creation selected on the part tab of the application options, exit the sketch. 2. Open the parameters dialogue and click Link. 3. In the open dialogue select the Excel file, select Link and enter the starting cell for the parameters. 4. Open the existing sketch, or create a new sketch. 5. Construct the geometry (sketches or features), referring to the names of the parameters as you build it.

12 6. If you forget to enter the value as a parameter, simply edit each feature and assign the parameter name to the value of the feature or sketch dimensions. Edit each feature or sketch dimension by their edit function or by the parameter table. 7. Make sure that if the part is used in an assembly, link the Excel spreadsheet to the assembly. Remember to be aware of the fact that linked Excel sheets are project specific. The Spreadsheet must remain in one of the specific project paths (but not a library path). It cannot be deleted like an embedded sheet. Figure 11: Linked Excel Parameters in Parameter Table

13 Linking Derived Parameters Using derived parameters in parts is the fundamental basis Skeletal Modeling. We will not discuss this exact topic, however we can take some of the basic concepts and apply them to traditionally constrained assemblies. Derived parameter linking does not have the computational horsepower that Excel provides. But there are no external document or files types to deal with. All data is inside one master file (native Inventor file). Advantages: Can be used to control many files at once Parameters can easily be changed to alter the assembly. No external files or connection problems with which to deal with (native Inventor file). Disadvantages: Project sensitive. The Master file must remain in one of the specific project paths (but not a library path). It cannot be deleted like an embedded sheet. Limited calculations and function available in the parameter dialogue The Master File The basic concept behind the Master Parameter File is that it is a native Inventor part file. The Master Parameter File contains only parameters, with no geometry. These parameters will be derived into all other part files. The derived part will be created based on these parameter names and values. This will allow changes in the Master Parameter File, and the other parts will update in turn. Creating the Master File Create a new part file and save it to a meaningful name, relative to your project. If you have the Sketch on New Part Creation selected on the part tab of the application options, exit the sketch. Open the parameters table. Create as many user parameters as required. If you forget to add a parameter, you can always add more user parameters at any time. Make sure to check the Export box of each parameter that you wish to export. Note: Only exported parameters get carried over to the derived parts. You can use other parameters inside the master file to help with complex calculations. Not checking the export box means they will not be included in the derived parts. However, their calculated values will still affect the other exported parameters.

14 1. You can use the limited Inventor functions to help develop simple calculations (+, -, *, /, Floor (), Ceil (), PI (), etc.). Remember that they are more difficult to use than their Excel counterparts. 2. When you have entered all of the user parameters, click Done. Notice in the browser, that no geometry has been created in the file. 3. Save and exit the file. Derive in the Master File 1. Create a new part file. Before you create any geometry, exit all sketches and click on the derive parts button. Select your Master file. You will see the Derived Part Dialogue Box. 2. Choose the items you want to derive into the new part file, in this case, the Exported parameters. Make sure that the symbol next to Exported parameters is a yellow +, and click OK.

15 3. Open the parameters table. You will see that the exported parameters now appear in this part. They are listed below the Users Parameters, with the title of the master file. 4. Construct the geometry (sketches or features), referring to the names of the parameters as you build it. 5. If you forget to enter the value as a parameter, simply edit each feature and assign the parameter name to the value of the feature or sketch dimensions. Edit each feature or sketch dimension by their edit function or by the parameter table.

16 6. Repeat this process for each of the files in the assembly that require to be linked. Have many similar parts in an assembly? Instead of deriving the Master into several different parts, make one part. Save Copy As to a new name. Open the new part. This maintains the link to the Master file. Now you can adjust the dimensions or values as necessary. This prevents from repeating the derived workflow over and over again. How do I derive the Master File after the geometry has been created? You can derive the Master file into the part file after geometry has been created. All you have to do is open the file, drag the End of Part marker to the top, and derive in the Master file. Once the Master file has been derived in, drag the End of Part marker back to the bottom. You can now adjust the dimensions or values as necessary. Figure 8: Moving the "End of Part" Marker Creating the Assembly File 1. After all parts have been linked, create the assembly. 2. Conventional constraint techniques may be used. If you have a simple assembly, then the process is complete. If you have a complex assembly that, requires one of the parameters that is in the Master file, then you will need to link the Master file to the assembly. 3. Open the parameters table. Click on the Link button. The normal File Open dialogue is displayed. Change the file filter. Select the drop down arrow, you will notice you can now link part files. Select the Master file and the exported parameters will be copied into the assembly file. You can now refer to them in the assembly file and they will update with the Master file.

17 4. Edit each feature or sketch dimension by their edit function or by the parameter table. Adjust the dimensions or values as necessary. 5. When you have adjustments to the parameters, click Done, Update the assembly, and save the file. Making changes to the Assembly Making changes to the assembly is easy. Open the Master file, and open the parameters table. Change the parameter values as necessary, then click Done. Save the file and then update the assembly. A double update or rebuild all may be required if the assembly is a very complex one. Conclusion Each workflow has its advantages and disadvantages. Both can help increase productivity, especially when changes have to be made. Practice using both workflows. Evaluate which one works for which parts and assemblies. Want to Learn More? Sean Dotson Look under the Tutorial s Tab Control Your Autodesk Inventor Data with Linked External Parameters Linked & Embedded Parameters - Part One Linked & Embedded Parameters - Part Two Linked & Embedded Parameters - Part Three Material Reference: Autodesk Inventor Help File Sean Dotson - Control Your Autodesk Inventor Data with Linked External Parameters, Autodesk University 2003, MA43-2