Friday, August 5, 2011

Using and Understanding Parameters in Autodesk Inventor - Part 1

Platform: Autodesk Inventor Professional

Level of difficulty: Beginners


Author: Ndianabasi Udonkang

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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.


Figure 1

The Parameters dialog box is shown below:


Figure 2


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.
  • Figure 3

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 -