Platform: Autodesk Inventor Professional

Level of difficulty: Beginners

Author: Ndianabasi Udonkang

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**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 parameter**s." 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 - |

can you use the parametrs used in part files... in the assembly files as well..

ReplyDeleteex:

i have 'l1x' in part1...

can i use 'l1x'to mean the 'l1x' in part1 also in the assembly?

The best advice I can give you is that you should endeavour to keep the parameter names unique. Especially if the names will be used in the same parameter table. For example, if "|1x" exists in part1 and also in assy1, then you would not be able to link the same "|1x" from part1 into assy1 and vice versa. In conclusion, the parameter table of each file (part file or assy file) is independent and can contain the same parameter names, provided you do not attempt to import or link those non-unique names into a parameter table that already contains the same names.

DeleteI have imported some parts from autocad 2011 with out using sketch command. In this case, is it possible to change dimensions using fx parameters provided in autocad inventor?

ReplyDelete(or)

How to establish fx parameters for imported objects to edit using formulae.

It will be very useful to my work.

AutoCAD, by default, doesn't design with parameters like Inventor does, so I doubt if you will be see any parameters in the Parameters dialog box for the imported model.

DeleteIf you need to import an AutoCAD model into Inventor, I will advise that you, first of all, open it with Autodesk Inventor Fusion (a free application). With Fusion, you can save the model as a "Fusion Edited DWG" which Inventor can easily recognise.Inventor recognises features/parameters created in Inventor Fusion, and vice versa.

You cannot establish parameters for the existing features that were imported with the AutoCAD model, but an changes to the model done on Inventor, thereafter, will be parametric. Cheers!