Designing with Parameters in Autodesk Inventor

Designing with Parameters in Autodesk Inventor
PDHonline Course G320 (4 PDH)
Designing with Parameters
in Autodesk Inventor
Instructor: Chad A. Thompson, P.E.
PDH Online | PDH Center
5272 Meadow Estates Drive
Fairfax, VA 22030-6658
Phone & Fax: 703-988-0088
An Approved Continuing Education Provider
Designing with Parameters in Autodesk Inventor
Chad A. Thompson, P.E.
Table of Contents
Introduction......................................................................................................................... 1
Basic Parameter Concepts................................................................................................... 2
Renaming Parameters ......................................................................................................... 5
Using Document Settings with Parameters......................................................................... 7
Using Parameters in Equations ........................................................................................... 9
Reference Parameters........................................................................................................ 11
User Parameters ................................................................................................................ 12
Parameter Units................................................................................................................. 15
Linking Parameters from Other Inventor Files................................................................. 18
Linking Parameters From Spreadsheets............................................................................ 20
Parameters in Assemblies ................................................................................................. 21
Case Study #1: Determining the Safety Factor of a Plate in Tension.............................. 22
Case Study #2: Calculating the Velocity of a Vehicle..................................................... 26
Case Study #3: Determining the Equilibrium Position of a Spring-Loaded Assembly... 28
Case Study #4: Driving a Cylinder Design with a Spreadsheet....................................... 33
PDH Course G320
Autodesk Inventor is a parametric CAD application, meaning it makes use of editable
parameters to build 3D models. As you create a model, parameters are created behind the
scenes which store necessary values for building the model. These parameters can be
changed after initial modeling to modify the model, they can be used in equations to
create relationships between parameters, or they can be shared between files.
This course will discuss many topics involving Inventor parameters, including using
parameters in equations, giving parameters meaningful names, creating user parameters,
and sharing parameters with other Inventor files as well as with spreadsheets.
A basic level of proficiency with Inventor is presumed for students taking this course,
especially an understanding of how to create parts and assemblies. Access to the
software while taking the course, while not required, is highly recommended in order to
follow along with the concepts discussed. Any version of Inventor is fine for this
Inventor 2010 is used in this course to illustrate examples, but the concepts discussed
here are applicable to any previous version of Inventor, and presumably future versions
as well. For the purposes of this course, differences between Inventor 2010 and previous
versions are minor, and will be noted where appropriate.
At the end of this document are several case studies where many of the principles
discussed here are applied in simulated real-world scenarios.
© Chad A. Thompson, P.E.
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Basic Parameter Concepts
In the part below, a rectangular block has been created by extruding a sketched rectangle.
As this feature is created, each of the defining dimensions is set up automatically by
Inventor as a parameter. We can see these parameter definitions by opening the
Parameters dialog box. To access this dialog box, go to the Manage tab, and in the
Parameters panel, click the Parameters tool button.
In versions of Inventor prior to 2010, the Parameters dialog box is accessed by clicking
the Parameters tool button in the panel bar.
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Note that, in a part file, you must be out of sketch mode to access the Parameters tool.
Looking at the parameters in the Parameters dialog box, we can see the model
parameters that Inventor has automatically created for the rectangular block above.
Each of the parameters has been assigned an arbitrary name of the format “dn”. We can
see each of the three values we used to create the rectangular block assigned to a
parameter name. (The d3 parameter was set up for the taper angle of the Extrude feature
that was created.)
If we return to the model and change a dimensional value, we see this change reflected in
the Parameters dialog box.
We can also change a parameter right in the Parameters dialog box, then update the
model to reflect the change. Simply click in the Equations field for the appropriate
parameter and type in the new value.
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When a parameter is modified in this manner, a manual update must be performed on the
model to reflect the change. To do this, click the Update tool in the Quick Access toolbar
at the top of the Inventor window.
In versions of Inventor prior to 2010, the Update tool is found in the Inventor Standard
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Renaming Parameters
The arbitrary “dn” convention used by Inventor when assigning parameter names can
become confusing. The parameter list can grow quickly as additional features are added
to an Inventor part, and keeping track of critical parameters can become unnecessarily
burdensome if this naming convention is maintained.
Inventor gives us the ability to assign more meaningful names to our parameters, thus
allowing us to reference the parameters more readily later on. This can be very useful
when changing parameter values in the Parameters dialog box, or when using parameter
names as variables in equations.
Continuing with our rectangular box from the previous section, let’s open the Parameters
dialog box to give the critical parameters in our model more meaningful names. To
rename a parameter, simply click in the field in the Parameter Names column and type
the new name. We can rename all three parameters which define the critical dimensions
of our rectangular block.
There are some limitations on what we can name our parameters. Parameter names
cannot have special characters in them, including spaces. There are also a few other
expressions that are reserved by Inventor for other purposes which cannot be used as
parameter names. Inventor will give you an error message if you attempt to give a
parameter an invalid name.
Parameter names are also case-sensitive. For example, using the expression “height” or
“HEIGHT” in an equation would not appropriately reference the first parameter on our
list above.
Prior to Inventor 2010, the method above was the only way to rename a parameter. You
would create the parameter in the model, Inventor would assign an arbitrary name to the
parameter, and then you would rename the parameter through the Parameters dialog box.
There is a quicker method in Inventor 2010 which allows you to give the parameter a
meaningful name as you are creating it. When you are entering a dimension value,
simply use the format <parameter name>=<value>.
For example, in our rectangular block example, if we create another sketch and add a
dimension to that sketch, we can type the new dimension value as shown.
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This functionality works in feature creation dialog boxes as well. For instance, we can
create a cut extrude feature on our part using the above sketch, and use the same
technique to rename the parameter defining our extrude depth, as shown below.
If we open the Parameters dialog box, we see the new parameters with the designated
names we assigned to them as we created the new feature.
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Using Document Settings with Parameters
There are a few settings in Inventor you should be aware of when working with
parameters. To access these settings, on the Tools tab, in the Options panel, click
Document Settings.
In versions of Inventor prior to 2010, access Document Settings from the Tools menu.
In the Document Settings dialog box, under the Units tab, are the default unit settings, the
dimension display setting, and the input display setting (not found in versions prior to
The Units settings determine the default units for parameters. These are typically set up
in your Inventor template files and are brought into a new file when the desired template
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for the new file is selected. However, these settings can be changed at any point after the
file is created as well. We will discuss units further later in the course.
The Dimension Display setting can be set to show model dimensions as values, parameter
names, or both. For instance, setting the dimension display for our rectangular block file
to Display as expression results in the model dimensions being displayed as shown.
Setting the Input Display to Display as expression results in an expression being
displayed in the Edit Dimension dialog box as shown. Again, this option is not available
in versions of Inventor prior to 2010.
When overwriting an existing expression for a dimension value while in this display
mode, it is not necessary to type the parameter name unless you are changing it.
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Using Parameters in Equations
A huge advantage in parametric modeling is the ability to use equations to drive the
values of our parameters. These equations can make use of mathematical operators and
functions, and can also use other parameters as variables.
Mathematical functions that Inventor recognizes are listed below.
pow(expr1; expr2)
For more details on these functions, consult the Help menu in the Inventor application.
As a simple example of using an equation, let’s make the length of the cut in our
rectangular block equal to one-fourth of the total length of the block. We can do this by
entering an equation for the CutLength parameter. One way to do this is to open the
Parameters dialog box and edit the Equation field for CutLength as shown.
Note the results of the equation shown in the Nominal Value column. (The ‘ul’ at the end
of the equation stands for unitless, and indicates that the ‘4’ term in the equation has no
units associated with it. The ‘ul’ doesn’t have to be typed in. Inventor fills this into
equations automatically where it is needed. We will discuss units further a little later.)
We might set up this scenario if, for instance, we’re pretty sure we want the length of the
cut to be one-quarter of the total block length, but we’re not sure what the final block
length will be. If we want to experiment with different block lengths as our design
progresses, we only have to change the Length parameter and the CutLength parameter
changes automatically to accommodate it.
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An equation can also be assigned to a parameter by entering the equation as the value for
a sketch dimension or as the distance in, say, an extrude feature. For instance, if I want
the parameter CutDepth to always be one-half of CutLength, I can edit the sketch for the
extrude feature and enter the appropriate equation for the dimension value, as shown.
Below, note again the automatic addition of the ‘ul’ term. Also note the ‘fx:’ symbol in
front of the parameter name, indicating that the value of the parameter is calculated from
an equation.
The usefulness of the ‘fx:’ symbol becomes more obvious if we change our dimension
display setting to Display as value. We can see below that if the symbol were not there,
it would not be obvious that the value of the dimension was the result of an equation.
We will look at more examples of parameter equations later in the case studies.
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Reference Parameters
Reference parameters are created when driven dimensions are placed on a sketch. For
instance, if we open the sketch for the extruded cut in our rectangular block, we can place
a driven dimension (indicated with parentheses) as shown.
If we open the Parameters dialog box, we can see the driven dimension represented as a
reference parameter.
This parameter can be renamed or referenced in an equation just like the model
parameters we have looked at. Note, however, that the equation field is in gray,
indicating that it is not directly editable.
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User Parameters
User parameters are not created by placing dimensions in a sketch or creating features.
Instead, they are created directly in the Parameters dialog box. They can be used in
equations or referenced in sketches and features just like other parameters we have
looked at.
To create a user parameter, open the Parameters dialog box and click the Add button.
This will create a new line in the User Parameters area, where the name and the equation
for the user parameter can be entered.
To show user parameters in action, see below a rectangular plate with a single mounting
hole in one corner. We would like to use the parameters we have set up to create a
rectangular pattern so that each corner has an identically placed hole.
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We will begin by opening the Parameters dialog box and creating two user parameters as
These user parameters will be used to set the spacing for our rectangular pattern. As the
Length and Width parameters vary, the pattern spacing will change accordingly so that
the holes always remain in the same place relative to the edges.
In the rectangular pattern dialog box, we simply need to fill in our user parameter names
in the pattern spacing fields. We could type in the names manually, but to save some
keystrokes, we can use another technique. Highlight the value in the field, then click the
flyout arrow and select List Parameters as shown.
This will display a list of all the parameters that have user-created names. We simply
need to select the appropriate parameter name from the list and it will be filled in
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Repeat for the spacing in the other direction, and we have linked our pattern spacing to
the user parameters.
At this point, perhaps we might want to save this part as a template or an iPart. For each
new plate size, we need only change the Length and Width, and the hole pattern updates
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Parameter Units
Each Inventor parameter has either a type of unit, such as inches or degrees or pounds,
assigned to it, or it is unitless, such as a parameter specifying the number of occurrences
in a feature pattern. Also, each term in a parameter equation must have the units
The units for model parameters are determined by the default units settings, which we
looked at previously in the Document Settings. If no units are specified for a parameter
value, the default units are assumed. For instance, if a file has inches set up as the default
length units, and we enter a value of ‘14’ as a parameter value, Inventor will assume we
mean 14 inches, and ’14 in’ will be displayed in the equation field.
We can, however, still explicitly indicate alternate units for the value of a parameter. For
instance, even if a parameter is set up with inches as its units, we can enter ‘150 mm’, and
Inventor will understand that we mean 150 millimeters. Of course, the alternate units
must still be the same type of unit. For instance, in the previous example, inches and
millimeters are both units of length.
Looking again at the Parameters dialog box for our rectangular plate, we can see that the
Units fields for the Model Parameters are gray, while those for the User Parameters are
The Model Parameters units cannot be edited from the Parameters dialog box. As we
discussed, these units are set by the default unit settings in the Document Settings dialog
We can, however, edit the units for our user parameters. By simply clicking in the Unit
field for a user parameter, we bring up the Unit Type dialog box, where we can select
alternate units for the parameter.
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If we change the units for our two user parameters to millimeters, note below that the
value for each of the parameters is now displayed in millimeters.
Inventor also understands unit prefixes. Shown below are the prefixes which can be used
when specifying parameter units.
"exa" "E"
"peta" "P"
"tera" "T"
"giga" "G"
"mega" "M"
"kilo" "k"
"hecto" "h"
"deca" "da"
"deci" "d"
"centi" "c"
"milli" "m"
"micro" "micro"
"nano" "n"
"pico" "p"
"femto" "f"
"atto" "a"
For instance, say we want a user parameter with units of kilo-pounds, or kips. Looking at
our default choices for force in the Unit Type dialog box, this is not one of the options.
We can, however, select lbforce, and then add a ‘k’ in front as shown to create our
desired units.
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We can also specify combinations of recognized units to create custom units, such as
rad/s (radians per second) or N m (newton-meters). Many of the units recognized in
Inventor are unrelated to the actual physical dimensions of the model. As we shall see in
the case studies later, though, they can still be quite useful.
The syntax for a unit must be entered exactly as it is shown in the Unit Type dialog box,
including the case. With a few exceptions, most units in Inventor are lower case. For
instance, for units of inches, Inventor recognizes ‘in’, but not ‘IN’ or ‘inches’.
Because Inventor understands and uses units, it also looks for agreement between the
units of a parameter and the resulting units of the equation for the parameter.
For instance, if I have a part with two parameters Length and Width, both with units of
inches, and I attempt to specify the distance for an extrusion with the equation
Length*Width, I get an error message as shown.
Note also that the equation entered in the field for extrusion distance is in red. As I am
typing an equation in either a feature dialog box, a dimension edition box, or the
Parameters dialog box, the text will show as red until the units of the equation are in
agreement with the units of the parameter.
© Chad A. Thompson, P.E.
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Linking Parameters from Other Inventor Files
An Inventor file can make use of parameters from other Inventor files. To set up this
link, open the file which will make use of the linked parameters, open the Parameters
dialog box, and click the Link button.
In the example above, a link has been established between the open file and three other
files. Parameters from each of the files have then been used in equations for the model
parameters of the open file.
When the second link above was established, the needed parameters were specified by
selecting them from a list, as shown.
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The icon before each parameter indicates whether the parameter is included or excluded
from the link. Clicking the icon for a parameter changes the parameter’s status.
Also, if we open up the linked file and look at its parameters, we see that in the Export
Parameter column there is a check placed in the boxes for the two parameters selected.
This indicates that these parameters are available to be referenced by another file. These
check boxes can be selected or unselected manually from within the Parameters dialog
If a parameter is chosen to be included during the linking process, and the Export
Parameter check box is not already selected for that parameter, the box will be selected
automatically, and a message will be displayed indicating that this has been done.
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Linking Parameters From Spreadsheets
In some cases it may be preferable to use a spreadsheet to maintain parameters for your
Inventor files. This may be due to the ease with which data can be manipulated within a
spreadsheet, the need for formulas which may be cumbersome or even impossible to do
within Inventor, the need to pass data to multiple Inventor files from a single source, or
the need for non-Inventor users to view or edit the design parameters.
The spreadsheet itself must be formatted properly so that Inventor can recognize the
contents as parameters. The data can start on any cell of the spreadsheet, and it can be in
rows or columns, but the rows or columns must be in a specific order, which is:
1) parameter name, 2) value or equation, 3) unit of measurement, 4) comment.
To link a spreadsheet, again click the Link button in the Parameters dialog box. With the
file type set to Excel Files, browse to and select the desired Excel file, specify the cell in
which the data starts, and choose whether you want to link or embed the file.
Choosing Link maintains a link to the external Excel file, and is typically used whenever
there is a need to maintain a separate file, such as if multiple Inventor files will access the
spreadsheet data, or if non-Inventor users need to access the data in the spreadsheet.
Choosing Embed copies and embeds the spreadsheet within the Inventor file, and no link
is maintained to the original external Excel file. Any changes to the data in an embedded
spreadsheet only affect the Inventor file in which the spreadsheet is embedded.
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Parameters in Assemblies
Thus far, we have only looked at parameters in part files, but Inventor assembly files
make use of parameters as well. Things like offset values for assembly constraints and
numbers of occurrences for component patterns are maintained as parameters in assembly
Parameters in assemblies are accessed in the same way as in part files, through the
Parameters dialog box, and the same principles apply for manipulating the parameters.
Assembly parameters have units, can be populated with equations, and can be linked
from other files.
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Case Study #1: Determining the Safety Factor of a Plate in Tension
While more advanced versions of Inventor have some sophisticated stress analysis tools,
here we will make use of the parametric functionality in basic Inventor to determine the
stress and safety factor for a part. We will also use parameters set up some guidelines for
how many mounting holes the plate needs based on the width of the plate. Since this is a
relatively simple model, it may be helpful to create your own Inventor part and follow
along with the steps below.
Let’s create a rectangular steel plate with its dimensions determined by parameters named
PlateWidth, Thickness, and Length as shown.
Let’s then create a sketch for a slotted hole in the plate using parameters named
SlotLength, SlotWidth, XSetback, and YSetback as shown, then make a cut extrude
through the plate using the sketch.
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Now we want to create a pattern of slotted holes using this initial hole as the basis, but
let’s first set up a parameter to automatically calculate the number of holes based on the
plate width using the following rules:
- If the width is less that 8”, there should be two rows of holes across the width.
- For a plate width of 8”, there should be three rows of holes
- For every additional 4” of width beyond 8”, there should be another row of holes.
Let’s create a user parameter called NumRows, which will be used when patterning the
slotted hole to create the desired number of rows. Examine the formula below to see how
the results meet the above requirements. (The floor function rounds the argument down
to the next whole number, and the max function returns the largest value from the list of
Think about the units for each term in the equation as well to see how the results are
unitless, as required by the parameter.
We can now create the pattern of slotted holes using the parameters we have set up.
Examine the Rectangular Pattern dialog box below to see how the parameters have been
Note the use of the NumRows parameter to set the number of occurrences for Direction 1.
Note also that the distance fields for both directions are too small to see the entire
formulas that have been entered here. In a situation like this, the Parameters dialog box
can be useful for seeing the entire formula, as shown below.
Here are the results of the feature pattern with the PlateWidth parameter set to 8 inches.
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If PlateWidth is changed to 6 inches, the pattern is recalculated automatically as shown.
Let us now say that that a tensile force is applied to the plate in the direction of its length.
To find the tensile stress in the plate, we need to first determine the minimum crosssectional area across the plate, which is the area through the slots. See below.
We will create a user parameter called CrossSection, with the equation shown below to
determine the cross-sectional area across the slots. Note again the units defined for the
parameter, in this case square inches, and how this agrees with the results of the formula.
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The value for the tensile force must be specified, and for this we will simply set up
another user parameter called TensileForce, with units of lbforce, and enter the desired
While advanced versions of Inventor capable of stress analysis can determine the yield
strength of an assigned part material, here we are assuming only basic Inventor
functionality. Therefore, we will set up the yield strength of the material as a manually
entered user parameter as shown. Note the use of psi (pounds per square inch) as the
units for the parameter. This is a standard unit of measure in Inventor.
Finally, we will set up one more user parameter as shown to calculate the safety factor for
the part.
We now have a parameter for the safety factor that is tied to the part geometry and to two
values which are entered manually, the material yield strength and the applied tensile
force. If any of these variables changes, the SafetyFactor parameter will be instantly
updated to reflect the change, eliminating the need to pull out a calculator to check the
safety factor every time any of these conditions change during the design process.
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Case Study #2: Calculating the Velocity of a Vehicle
Here we have a model of a wheel whose outside diameter has been set up using a
parameter called WheelDia, as shown below. (To create your own model and follow
along with this case study, there in no need to create any complex geometry. A simple
cylinder will do.)
Let’s say we are still in the design stage for our wheel, and the diameter may still change.
We would like to be able to quickly determine what the maximum velocity will be for the
vehicle which uses this wheel whenever the wheel diameter or the angular velocity of the
wheel changes.
Shown below is a user parameter for the maximum angular velocity of the wheel. Note
the use of rpm (revolutions per minute) for the units, which is a standard unit of
measurement in Inventor.
As it is shown here, MaxRPMs is simply a manually input value, but it could just as
easily be linked from another file, say the model of a drive motor.
Let us now say we want to calculate the maximum vehicle speed in miles-per-hour based
on our two values for the wheel diameter and the angular velocity. Even though we have
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only two variables to deal with, the manual calculation is quite laborious simply because
of all the conversion factors we need to employ to get from inches and RPM’s to mph.
The manual calculation would look something like this:
[(500 rev/min)*(10p in/rev)*(60 min/hr)] / [(12 in/ft)*(5280 ft/mile)] ≈ 14.9 mph
And, of course, if either our angular velocity or wheel diameter changed, we would need
to run through this calculation again to determine the new vehicle speed.
Let’s now set up a user parameter in Inventor called VehicleSpeed to calculate our vehicle
speed automatically. Here is what the formula looks like.
Something interesting is going on here. As we can see, the resulting value for our
parameter is about 14.9 mph, which is the same value we would get if we ran through the
manual calculation above, but the formula for our parameter doesn’t look much like the
formula for the manual calculation. (Note: the term ‘PI’ is a recognized mathematical
term in Inventor representing the unitless value 3.14159...)
To understand what’s happening, let’s think, not about units, but about the unit types.
Our specified units for the parameter, mph, could be though of in terms of unit type as
If we look at the terms in our formula in this same way, we get this:
Our formula works because its unit type is the same as that of the specified units for our
parameter, even though the units themselves are different. It’s the same concept as when,
say, we have a parameter with units set to millimeters, and we enter ‘1 in’ for the
equation. The value for the parameter is 25.4 (there are 25.4 mm in an inch) because
Inventor understands the relationship between millimeters and inches.
In this same way, Inventor understands the relationships between the different units in
our calculation for the vehicle speed. Indeed, if we want our vehicle speed expressed in
some other units, say meters-per-second, we simply need to change the units of the
parameter, and because the type of unit is still the same, the same formula is still valid.
Note here also that there is no standard Inventor unit for meters-per-second, but we were
able to combine two standard units to create a custom unit.
© Chad A. Thompson, P.E.
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Case Study #3: Determining the Equilibrium Position of a Spring-Loaded
Here we will simulate a spring-loaded assembly with an external force applied to it. We
will set up parameters to determine the equilibrium position of the assembly based on the
magnitude of the force and the properties of the springs.
Our assembly looks like this...
...and a cross-section of one of the cylinders looks like this.
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We wish to apply a force on the top surface of the upper plate, and based on the number
and properties of the springs, we want to know the resting position of the assembly.
Let’s first examine the part file for the spring. There are two pertinent parameters in this
file, the free length of the spring (i.e. the length of the spring with no applied force),
named FreeLen, and the spring constant (i.e. the force required per inch of spring
compression), named SpringConstant.
Note the combination of two standard parameter units, lbforce and in, to create a custom
unit for the spring constant.
(In this example, I have actually created a physical representation of the spring as a part
file, which adjusts in length based on the conditions in the assembly. This requires some
Inventor functionality that is beyond the scope of this course, namely adaptivity. I have
done this primarily for illustrative purposes. One could easily set this assembly up using
imaginary springs with no physical representation. In this case, the parameters above
could simply be created in the assembly file rather than linked from another file.)
The number of cylinders used in the assembly, and therefore the number of springs, is
determined by a parameter set up in the base plate file called NumCyls. This parameter
has been used to set the number of occurrences in a circular pattern of holes which are
used as pockets for the springs in the assembly.
The pattern of cylinders in the assembly is based on the hole pattern in the base plate.
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There are several physical dimensions in our assembly which influence the springs, and
parameters have been set up in the part files which we can use in determining our
assembly position. Below is a cross-section of the cylinder with representations of the
pertinent parameters.
Returning to the assembly, we can create links to all of the above parameters so they may
be referenced by equations in our assembly.
Looking at the cylinder cross-section, we can see that there are physical limits to how far
the cylinder can extend or retract, and therefore limits to our maximum and minimum
spring length. Let’s set up user parameters in our assembly to determine these lengths.
Examine the equations below to see how they make use of the parameters from the part
files to determine these values.
Next, let’s set up a couple of user parameters in the assembly to represent the forces
applied to the springs. The total force is made up of two components, the weight of the
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moving parts in the assembly, and the force applied to the top plate. Here are the
parameters for those forces.
(Even though Inventor calculates the weight of parts and assemblies based on assigned
materials, these weights cannot be utilized directly as parameters when using only basic
Inventor functionality.)
We now have enough information to determine the compressed length of our spring. We
are assuming our springs are basic linear compression springs, which follow Hooke’s law
F = k * x or x = F / k,
where F is the force applied to the spring, k is the spring constant, and x is the
compression of the spring.
The force on each spring can be expressed as (AppliedForce + TareWeight) / NumCyls,
so Hooke’s law can be restated in terms of our parameters as
x = ( ( AppliedForce + TareWeight ) / NumCyls ) / SpringConstant
As we determined previously, there is a physical limit to how short the spring can be, for
which we created the parameter MinSpringLen, so our maximum spring compression is
found with the formula FreeLen – MinSpringLen. We can now set up a parameter for the
compression of each spring as shown. (The min function returns the lowest value from
the list of arguments. Each argument is separated by a semi-colon)
The length of each spring under load can then be determined with the formula
FreeLen – SpringComp.
Again, however, there is a physical limitation to the maximum length of the spring,
which we set up as the parameter MaxSpringLen, so we can set up a parameter for the
actual spring length as shown.
© Chad A. Thompson, P.E.
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We now need simply to create an assembly constraint which makes use of this parameter
to correctly position our assembly. Again, the physical representation of the spring, as
shown here, is not really necessary. An imaginary spring could be used, and the
parameters representing the spring properties could simply reside in the assembly file.
Though it takes a little time to create the initial setup for a design like this, we now have
the ability to change a number of variables, including the properties of the spring, the
force on the assembly, the number of cylinders, and/or the geometry of the cylinders, and
see instantly how those changes affect the position of our assembly.
© Chad A. Thompson, P.E.
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Case Study #4: Driving a Cylinder Design with a Spreadsheet
Here we have a simplified representation of a pneumatic or hydraulic cylinder consisting
of four parts, a body, a piston, a rod, and a bushing
In an effort to minimize effort when experimenting with various bores, strokes, and rod
diameters, we would like to make use of our ability to link parameters between files.
We might at first think the best approach would be to set up our critical parameters in the
assembly file, then link to those parameters in each part file to define our geometry. In
fact, this is not allowed in Inventor. This creates a circular reference whereby the
geometry of a part would be defined by the assembly file, and in turn, the assembly file
would be defined by the geometry of the part.
Another option would be for our critical parameters to reside in the part files, and then
the parameters can be referenced between the part files as needed. This approach would
work, but it could quickly become confusing to keep track of which parameters reside in
which part files. For instance, in the case of our cylinder, is the parameter defining the
cylinder bore in our body file or in our piston file? And, of course, the more complex the
assembly becomes, the more confusing this situation could be.
This is an example of where a spreadsheet can come in handy. Below is a portion of a
spreadsheet worksheet where the critical dimensions of our cylinder have been defined,
as well as a few other values.
© Chad A. Thompson, P.E.
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For clarity, the shaded cells are values input by the user. Note the formatting of the
spreadsheet, as defined earlier in the section Linking Parameters from Spreadsheets.
Each part in the assembly is linked to this spreadsheet and makes use of the three
parameters which define our physical dimensions, BORE, STROKE, and ROD_DIA. For
instance, if we look at the main sketch defining the dimensions for the cylinder body, we
see the BORE and STROKE parameters in use.
The other two input values in the spreadsheet, PRESSURE and FLOWRATE are not used
to define physical dimensions in our model, but are used in combination with our
physical dimension parameters to calculate the values for EXT_FORCE, RET_FORCE,
EXT_TIME, and RET_TIME. Note also the combination of two standard Inventor units,
ft and min, for the FLOWRATE parameter to create a custom unit of measurement for
cubic feet per minute, since cfm is not a recognized Inventor unit.
A link has been created to the spreadsheet for each of the part files in the cylinder
assembly, as well as the assembly itself.
While no physical dimensions from the spreadsheet are used directly in the assembly file,
the link can still be handy so that the other calculated values can be viewed in the
Parameters dialog box without having to open the spreadsheet.
Another potential advantage to using a spreadsheet for Inventor designs is that it gives
non-Inventor users access to view or edit design parameters.
© Chad A. Thompson, P.E.
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