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Using and Understanding Linked Parameter in Autodesk Inventor

Platform: Autodesk Inventor Professional

Level of difficulty: Beginners


Author: Ndianabasi Udonkang

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This is the second lesson in our series about using and understanding parameters in Autodesk Inventor Professional. In the first lesson, we got ourselves familiarized with the general concepts on parameters. In case you missed the first lesson, read it here: Using and Understanding Parameters in Autodesk Inventor - Part 1.

LEARNING OBJECTIVES

At the end of this lesson, you should be able to:

1. Create user-defined parameters using Microsoft Office Excel.
2. Link the Excel spreadsheet document to a part or assembly file inside Autodesk Inventor.
3. Update an Inventor part or assembly file when changes have been made to the source spreadsheet file.

OVERVIEW

In Autodesk Inventor, a Microsoft Office Excel spreadsheet file can be used to create user-defined parameters which then can be linked to a part or assembly file. This way, a single Excel spreadsheet file can be reused across many Inventor files as the source for user-defined parameters. Excel spreadsheet files have the file extensions ".xls" for Excel 2003 documents, and ".xlsx" for Excel 2007 and 2010 documents. For you to understand this topic, it is required that you have a basic understanding of how equations are created in Microsoft Office Excel.

Linking parameters has an obvious advantage since you do not need to create the same parameters in each Inventor file you create. This is also the principle behind many features and standard parts including Thread features, Bolted Connections, gears, etc.

There is a major drawback in using external spreadsheet files as sources of user-defined parameters. Now imagine losing the spreadsheet files in unfortunate circumstances; this means you have also lost all the parameters that were stored in them, and your Inventor files will become useless! This is often the situation with people who play with their thread.xls file and find themselves unable to create thread features and bolted connections. So be careful and make sure that you backup your spreadsheet files.

So let us get started! The process of creating and using linked parameters in Autodesk Inventor will be divided into the following steps:

STEP 1: CREATE THE MICROSOFT EXCEL SPREADSHEET FILE

In creating an Excel spreadsheet file that will be linked to an Inventor file, a format must be followed. Just as the Parameters dialog box in Inventor, the parameters are arranged in rows and the parameter variables are arranged in columns. For such an Excel spreadsheet file, four variables are basically sufficient. They are:

1. The parameter name;
2. The parameter value;
3. The parameter units; and
4. The parameter comment.

For more about the different variables, check out this first lesson about parameters, Using and Understanding Parameters in Autodesk Inventor - Part 1. However, I will mention that you are not required to fill the Units column if the units of the parameters are the same as that of the template used in creating the Inventor file.

PROCEDURE:

1. Launch Microsoft Office Excel 2003, 2007 or 2010 through any means known to you. For Windows 7 and Vista users, go to Start Menu > All Programs > Microsoft Office > Microsoft Office Excel 200x.
2. In the Excel environment, create the spreadsheet shown below.
3. 
4. Save the file with the name "Linked_Parameters" in the project folder of the project you wish to use. For example, mine is saved in the Training folder – which is the folder for my active Inventor project (C:\Users\Ndianabasi\Documents\Inventor\Training).

STEP 2: CREATE A NEW INVENTOR PART FILE

Here you are going to create a new Autodesk Inventor part file.

PROCEDURE:

1. In Autodesk Inventor, create a new part file using the Standard (mm).ipt template. Pressing CTRL+N is a fast way of achieving this. The Standard (mm).ipt template is found on the Metric tab of the New File dialog box.
2. Use the Rectangle tool to create a rectangle over the center of the sketch.
3. Constrain the rectangle to be centered around the center of the sketch using the Vertical and Horizontal constraints. Finish the sketch and save the file as Linked_Parameters.ipt.
4. 

STEP 3. LINK THE SPREADSHEET FILE TO THE INVENTOR PART FILE

Here we are going to learn how to link the previously created spreadsheet file to the just created Inventor Part file.

1. On the Ribbon, go the Manage tab > Parameters panel > Parameters tool. Click on the Link button at the bottom of the Parameters dialog box.
2. 
3. On the Open dialog box, scroll down the project folder and select the Excel spreadsheet file Linked_Parameters.xlsx or Linked_Parameters.xls depending on the Excel version that was used.
4. At the bottom of the Open dialog box, change the Start Cell from A1 to A2. This value is changed because the actual parameter data starts from cell A2; the first row was used to define the column headers. Click the Open button.
5. 
6. The Excel parameters are now linked to the Parameters dialog box as shown below.
7. 
8. Click Done to close the dialog box.

STEP 4: MAKING USE OF THE LINKED PARAMETERS

In this section we are going to learn how to use the linked parameters inside the Inventor part file.

1. Double click Sketch1 on the Model Browser of Linked_Parameters.ipt.
2. On the Sketch tab > Constrain panel, click on the Dimension tool (Shortcut = D).
3. Click one of the horizontal lines and click below the line to place the dimension. The Edit Dimension box should be displayed to allow you edit the size of the dimension. If it does not come up, right click on the graphics area immediately and activate Edit Dimension on the context menu.
4. On the Edit Dimension box, while the dimensions to be edited are highlighted, click on the arrow pointing towards the right of the screen or right click the input area. Click List Parameters on the context menu.
5. 
6. The Parameters list box pops up with the three linked parameters. Click on Box_Length.
7. 
8. Click the green tick at the end of the Edit Dimension box to return the parameter.
9. Repeat step 2 to 7 and dimension the vertical line using the Box_Width parameter.
10. Click Finish Sketch on the Exit panel. Your unconsumed sketch should appear as shown below.
11. 
12. On the Model tab > Create panel, click on the Extrude tool (Shortcut = E). On the Extrude dialog box, highlight the Distance1 parameter and click the arrow pointing to the right of the screen. On the context menu, click List Parameters. On the Parameters list box, click Box_Height. Click OK to create the Extrude feature.
13. 
14. Save the file (CTRL+S).

STEP 5. UPDATING THE MODEL BY CHANGING THE VALUES OF THE PARAMETERS IN THE EXCEL SPREADSHEET FILE.

Here we are going to learn how to changes to the values of parameters in the Excel spreadsheet file are reflected on the part file.

1. Using Windows Explorer, navigate and open the Linked_Parameters.xlsx file saved in your project folder e.g. C:\Users\Ndianabasi\Documents\Inventor\Training\Linked_Parameters.xlsx.
2. Change the value of Box_Height parameter to 20.
3. Save and close the Excel file.
4. Return to the part file and glance up at the Quick Access Toolbar at the top of the application just by the left of the title bar and by the right of the Menu Browser. Inventor has detected the changes make to the Excel spreadsheet file and indicates that an update is necessary.
5. Click on the Local Update button on the Quick Access Toolbar as shown below.
6. 
7. The part updates accordingly.

CONCLUSION

I hope that the tutorial was beneficial. Drop a comment or contact me. Thanks for stopping by.

Using and Understanding Parameters in Autodesk Inventor - Part 1

Platform: Autodesk Inventor Professional

Level of difficulty: Beginners


Author: Ndianabasi Udonkang

Follow me on Twitter | Facebook

Whoa! It is nice writing another interesting article on Autodesk Inventor Professional. This time we are going to deep into the world of parameters - the engine house of Inventor Professional. Of course, by now, we already know that Autodesk Inventor Professional is a 3D feature-based parametric modelling application. For avoidance of confusion, Inventor is said to be feature based because each modification to a component is regarded as a feature. So in a design workflow for a component, you would most likely make use of extrusion, swept, lofted, revolved, threaded, hole, rib, fillet, shell, and chamfer features. If you are also experienced with surface modelling, you would likely use features like sculpt, thicken, patch, and trim. These features are usually conspicuously listed on the model browser in the order in which they are added to the design (though they can be reordered as long as it does not affect their dependencies) and the features could be modified at any time as long the modification would not be detrimental to dependent features.

Inventor is called a parametric modeler because the sizes of the features and their relationship with each other; the relationship of one part to another in an assembly; the forces, pressures, and moments applied for stress analysis; and the forces, torques, velocity, and acceleration applied in dynamic simulation environment are all parameters! These parameters are actively involved in controlling the shape and
behavior of the part or assembly being created.
So the power of Inventor Professional lies in its use of parameters for controlling the models, so that there is associativity between the model and the numbers controlling any particular feature on a model. From the first line drawn to the last engineering analysis carried out on a model, parameters are intelligently quot;harvested" by Inventor. As an engineer, these parameters are the data you need.

Depending on the design intent, you may want to create "user-defined parameters" whose value could be obtained from just ordinary numbers, simple mathematical equations, or complex equations embedded with other parameters. Such
complex equations could be found in the designs of machine elements like gears, v-belts, sprockets, fasteners, etc.

Every parameter must have:

• A name;
• A unit;
• An equation; and
• A value.
• Others are optional.

By default when you begin a new part, dimensions (I prefer to call them dimensional constraints) are added by you to

the design. These dimensions are parameters and they are named from d0 upwards. Parameters that are created automatically by the application as you add dimensional constraints, extrusion height, hole depths, etc are called "model parameters." Those added manually by the user are called "user-defined parameters." Other types of parameters might be added if you use Stress Analysis and Dynamic simulation environments.
So how can you bring up these parameters and play around with them? Simple! With at least one component opened, go to the Ribbon > Manage tab > Parameters panel > Parameters tool.

The Parameters dialog box is shown below:





The parameters are listed as records (rows) in the dialog box while the Parameter Name, Unit/Type, Equation, Nominal Value, etc are arranged in columns.

PARAMETER NAME

• The parameter name is a unique identifier assigned to each parameter.
• For a particular part, no two parameters can have same parameter name.
• Model parameters are usually named d0, d1, d2, and so on. These could be renamed but they remain model parameters.
• You cannot begin a parameter name with a number. That is, "1stDia" is not allowed as a parameter name.
• If the name of a user-defined parameter is made up of more than one word, spaces are not allowed between the words. That is, the name "Hole Dia" is not permitted since there is a space between Hole and Dia. In this case, it is appropriate to use underscores (_) to separate the words e.g. "Hole_Dia".
• Another way of writing parameter names could be by beginning the first word with a lower-case letter and capitalizing the first letter of subsequent words that make up the parameter name (a convention adopted by most programmers) e.g. "holeDia", "filletRadius", "forceOnComp", etc.
• When you point at a parameter name on the Parameters dialog box, a tooltip displays the parameters, sketches and features that currently consume (or make use of) the parameter. For example d4 is consumed by d5,
  
  d6, and 3D Sketch1.
• 

UNITS

• The Unit/Type column is used for specifying the units for the parameters.
• The unit cannot be modified for model parameters. They depend on the default unit that was specified during installation or the template that was used for creating the model.
• For user-defined parameters, the unit/type can be modified during creation.
• For linear values, you might use unit types like millimeters, inches, or meters (mm, in, or m).
• For angular values, you might use unit types like degrees, radians, or gradient (deg, rad, or grad).
• When a number does not have a unit, then the unit type is unitless (ul). Such unitless parameters could be used for
  
  specifying the number of occurences in a pattern.

EQUATION

• The equation column is used for calculating the value of a parameter.
• The equation for a parameter could vary in complexity from a simple number to a simple algebraic equation to a
  
  complex equation involving trigonometry ratios, internal parameters, and other functions.
• Examples of equations that could be used are:
• d0 = 20 mm
• Hole_Depth = 4 ul (20 ul * d0 – 7 ul )
• tipDia = pitchDia * cos (PI / Z) + 2 ul * toothHeight
• where PI is an internal parameter for the constant, pi.
• You will encounter an error if you try to reference a non-existing parameter in another parameter. For example in
  
  the parameter tipDia shown above, if pitchDia, toothHeight or Z has not been defined
  
  previously, an error will be encountered.

ALGEBRAIC OPERATORS SUPPORTED BY INVENTOR

The following table lists the algebraic operators supported by Inventor.

OPERATOR	DESCRIPTION
+	Addition
-	Subtraction
%	Floating point
*	Multiplicatin
/	Division
^	Power
(	Expression delimiter
)	Expression delimiter
;	Delimiter for multi-argument functions

UNIT PREFIXES SUPPORTED BY INVENTOR

The following table lists some prefixes supported by Inventor.

PREFIX	SYMBOL	VALUE
deci	d	1.0e-1
centi	c	1.0e-2
milli	m	1.0e-3
micro	micro	1.0e-6
nano	n	1.0e-9
deca	da	1.0e1
hecto	h	1.0e2
kilo	k	1.0e3
mega	M	10e6
giga	G	10e9

FUNCTIONS SUPPORTED BY INVENTOR

The following table lists the supported functions in Inventor.

SYNTAX	RETURNS UNIT TYPE	EXPECTED UNIT TYPE
cos(expr)	unitless	angle
sin(expr)	unitless	angle
tan(expr)	unitless	angle
acos(expr)	angle	unitless
asin(expr)	angle	unitless
atan(expr)	angle	unitless
sqrt(expr)	unit^1/2	any
sign(expr)	unitless	any (returns 0 if negative, 1 if positive)
exp(expr)	unitless	any (Return exponential power of expression)
floor(expr)	unitless	unitless (Next lowest whole number.)
ceil(expr)	unitless	unitless (Next highest whole number.)
round(expr)	unitless	unitless (closest whole number.)
abs(expr)	any	any
max(expr1;expr2)	any	any
min(expr1;expr2)	any	any
ln(expr)	unitless	unitless
log(expr)	unitless	unitless
pow(expr1;expr2)	unit^expr2	any and unitless, respectively
random(expr)	unitless	unitless
isolate(expr;unit;unit)	any	any

ORDER OF ALGEBRAIC OPERATIONS

The following table shows the algebraic operations in descending order.

OPERATION	SYMBOL
parentheses	()
exponentiation	^
negation	-
multiplication or division	* or /
addition or subtraction	+ or -