Skeleton Modeling Manual

Skeleton Modeling Manual
Last edited: February 13, 2015
GEA Process
Engineering
PE CAD Operation
DAWN@gea.com
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Table of Contents
1. Introduction...................................................................................................................................3
1.1 How to use this manual .......................................................................................................3
1.2 The Purpose..........................................................................................................................3
1.3 Skeleton Modeling Workflow ..............................................................................................4
2. Creating Master Skeleton ..........................................................................................................4
2.1 To start Creating Master Skeleton...........................................................................................4
3. Creating Parameters...................................................................................................................6
To open the Parameters Dialog..........................................................................................................6
To Link Numeric Parameters from a Spreadsheet.............................................................................6
Create a parameters spreadsheet ....................................................................................................6
4. Creating Model using Derived Tool..........................................................................................9
To derive a part file:...........................................................................................................................9
To Create an Assembly....................................................................................................................10
Use Move to Origin command.........................................................................................................11
5. Creating Model using Multi Solid Body..................................................................................11
Make Components ...........................................................................................................................12
Workflow: Make Components from Solid Multi-Body part .......................................................13
Post - Make Component considerations ......................................................................................14
6. Summary ....................................................................................................................................15
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1. Introduction
1.1 How to use this manual
As you go through the manual, you will encounter different types of font styles to
emphasize a point, or a command. It is worth to know that there are some words in
hyperlink that will open a browser. In the browser, you can play a video to guide you
about a certain topic.
1.2 The Purpose
The purpose of this manual is to learn and use an efficient way of creating and
managing large assemblies through Skeleton Modeling using Autodesk Inventor. It
is a technique that facilitates centralized design criteria and creates components that
reference those criteria. This is also popularly known as Top-Down Design. In other
words, it is a process of creating a framework for a complex assembly, made of
components; via a single part file (a skeleton made of sketches).The skeleton is then
derived into several new part files where features are created. These parts are then
easily constrained in an assembly file as each part’s origin is the same. What drives the
change or revision in the assembly will be coming from the sketch geometry of the
skeleton part file (master part).The application of this technique is limited only by your
imagination.
Note: It is highly recommended to use the common origin workflow to derive shape and
position to your new components. Use the position independent workflow to derive shape
only. With position independent components, changes to the position of sketch geometry in
your layout do not require component revisions.
The user skill level is intermediate. It means that the Inventor user has a good
experience in part and assembly modeling, sketching, use of parameters and derived
parts. If you are not familiar with these topics, I highly suggest taking some time to
understand the fundamentals before you continue any further.
To guide you about the basics requirements of skeleton modeling, here are
some recommended videos (click the hyperlinks)
• Creating Sketches, Dimensions, and Constraints
• Defining Parameters
• Deriving Components
Before you start working on anything, you need to consider some solid
strategies about how do you intend to build the assembly model. First, begin with the
end in mind, means that you need to picture the finished product even before you start
creating a model. This is very important so that you can plan your master sketch,
whether you may need more than one master sketch to drive your sub-assemblies. As
you go along with the basic knowledge of skeleton modeling, you will create more than
one master sketch to simplify the complex structure of an assembly. For now, let’s get
started creating a skeleton modeling with a single master sketch.
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Here are some of the steps to create a Skeleton Modeling;
1.3 Skeleton Modeling Workflow
1. Creating Master Skeleton - create a single part model, called the skeleton,
consisting of the base sketches. These sketches reflect the layout of the
assembly components. Position the sketches to reflect the position of the
components in the assembly.
2. Creating Parameters - establish all critical parameters in the skeleton part. Be
sure to name the parameters appropriately and mark them for export. Use
Excel spreadsheet to link to the model.
3. Creating Model – there are 2 methods 1.) Use Make Part, from within your
layout, to create a component in your target assembly. Select the sketches,
work geometry, features, and bodies to derive into the component. The new
component is grounded at the assembly origin. 2.) Use Derived Component to
create the part model using the master skeleton.
4. Assembly – 1.) Use Make Component of your part model (skeleton) to
generate the solid bodies as component parts to a new assembly. 2.) use the
normal way of creating an assembly using the derived components.
2. Creating Master Skeleton
A Skeleton part file can contain of any type of elements in any mix. Typical
information created in a skeleton file can be:
• Sketches – defines the basic concept of the final product or are used as a
layout of different areas.
• Work Geometry – defines important connection points, axial directions and
work planes that define levels or partitions.
• Parameters - defines important values for sizing components, angles for
placements and other known design values.
• Solids – defines volumes for final assembly as a single part or for defining
subareas of the design. These are considered as features at the start.
2.1 To start Creating Master Skeleton
1. From the Get Started ribbon, Launch group, create New and choose the
Standard.ipt then click the Create button at the bottom right corner of Create
New File dialog box. Shortcut key is Ctrl + N.
2. Click Create 2D Sketch, then select a work plane to create sketch
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Figure 1 - Sketch Model
A good practice of sketching is to create multiple sketches for each part feature
or component model instead of creating a single sketch, that can complicate a
large assembly. This will help you focus on which sketches to derive when you
make your part component. The rule of sketch is to KEEP IT SIMPLE. See the
Figure 1 about how a master sketch part was created. Make sure to rename the
sketch features such that will make sense pertaining to the part component of
the assembly.
3. Save the sketch file as Skeleton.ipt.
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3. Creating Parameters
Parameters are created when you define a sketch dimension, add an assembly
constraint or create a feature. They are given a default name with "d" and numbered in
sequential order such as d0, d1, d2 and so on.
If you have not used parameters before, you will need to review Understanding User
Parameters (click the link). When working with parameters, it is a good practice to link
the skeleton part model to an excel spreadsheet. In this way, you control all the input
spec size in one source, excel spreadsheet. If you have not done any linking of
spreadsheet to the parameters before then you will need to review this video about
Linking Spreadsheet Parameters.
To open the Parameters Dialog
1. On the Ribbon, click Manage tab | Parameters panel | Parameters
or from the Quick Access Toolbar
Figure 2 – Parameters from Ribbon and Quick Access Toolbar
2. Do any of the following:
• To filter the display of parameters, select a filter from the Filters list .
• Expand or collapse the Model Parameters list and the User Parameters list.
• To delete a parameter, right-click on the parameter row and select Delete
Parameter.
• Right-click and select Copy/Paste or use the Ctrl+C and Ctrl+V shortcut to
copy and paste values within the Parameters dialog.
To Link Numeric Parameters from a Spreadsheet
If you use the same parameters in many models, you can define parameters in a
Microsoft Excel spreadsheet. You can embed or link to the spreadsheet from assembly
or part models.
Create a parameters spreadsheet
In Microsoft Excel, create a spreadsheet with the following format:
• The data can start in any cell of the spreadsheet. If the data does not start
in cell A1, specify the data start position in Inventor when you link or
embed the Excel file. If you use a column header name in a cell, do not
specify that cell as the data start position.
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• The data items can be in rows or columns, (let us use columns) but they
must be in the correct order: parameter name, value, or equation, unit of
measurement, comment.
Note: The order of the data in Excel differs from the order in the Inventor
Parameters dialog box.
• The parameter name and value are required; the other items are
optional. The cells associated with parameter name and value cannot be
blank.
• If you do not specify the units of measurement for a parameter, the default
units for the model are assigned when you use the parameter. To create a
parameter without units, enter UL in the units cell.
• You can include column or row headings or other information in the
spreadsheet, but they must be outside the block of cells that contains the
parameter definitions.
Here is an important thing to remember when linking to an excel spreadsheet. From
the Parameters dialog box, when you click the Link button, the Open dialog box is
opened as shown in Figure 3. In the Start Cell field, key in the correct cell number
where you started your variable name. For example, key in A2 (See Figure 4 – Excel
Spreadsheet) from the example of spreadsheet below. Select Embed as the option.
Figure 3 – Open Link dialog box
Below image is an example of an excel sheet of a component assembly. The
important factors required in the spreadsheet are the variable name and the value.
You can include a unit of measure and comments/remarks as an option but it is
advisable to include these options. In the value cell, you will need to key-in hard
numbers or cell formulae.
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Figure 4 – Excel Spreadsheet
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4. Creating Model using Derived Tool
Derived parts are base solids that are linked to the original feature-based part (in this
case, our skeleton model). Modifications to the derived part in the form of additional
features are allowed; in fact this is our approach in building a part model. Original
features such as skeleton sketches are modified in the parent part and changes to the
parent part are moved to the derived part upon save and update.
To derive a part file:
Create New File to start creating a model or click New from the Application menu.
Select the Standard.ipt template. If by default it opened up a sketch environment, click
the Finish Sketch to exit. Delete the sketch feature (normally Sketch1).
In the 3D Model tab ribbon, go to Create panel and click Derive command or
In the Manage tab ribbon, go to Insert panel. Click Derive command then an Open
dialog box will be shown. Select the master skeleton that you created from (2.1
number 3) Skeleton.ipt.
Figure 5 – Derive Part dialog box
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In the Derive Part dialog box, leave the marked default options as shown in Figure
5. In the Derive style, leave the default option to Maintain each solid as a solid
body. This will be useful when creating Multi-Body parts. You have the option to
select a sketch or more sketches, work geometry, solid body, user parameters or other
relevant features.
You can click a status icon next to an individual object and toggle the status options.
Selects element for inclusion in the derived part.
Excludes element in the derived part. Items marked with this symbol are ignored in
updates to the derived part
Select OK to finish. Create features (extrude, revolve, sweep, etc.) to make your
solid component part.
After the part modeling is finished, create a new assembly to place your component
parts. We will use 2 methods of assembly modeling.
To Create an Assembly
i. From the Application Option, select New. Select Standard.iam template
from Create New File dialog box.
ii. From the Ribbon | GEA CAD Tools tab | Insert panel | Assembly Insert
iii. From the Assembly Insert dialog box, browse the folder of components and
select the parts or subassemblies accordingly. Check the Ground option.
Select the Insert at Origin button to place all the components. Close.
Figure 6 – Assembly Insert dialog box
Watch the Assembly Insert video for more information.
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Use Move to Origin command
There are times wherein you have to add new components to an assembly. In
this case, use the Move to Origin command from GEA CAD Tools. You can
place multiple components and move them together to the origin.
On the ribbon, select GEA CAD Tools tab | Insert panel | Move to Origin
command.
You need to select the components first before selecting the Move to Origin
command. It will prompt you to move and ground the component(s). Select Yes
to start the process. If you select No, the component(s) will move to origin but it
will not be grounded.
Watch the Move to Origin video for more information.
5. Creating Model using Multi Solid Body
Figure 7 – Solid Bodies
The first feature that you create in your part file (skeleton) will automatically create a
new body.
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Figure 8 – New Solid
Creating a multi-body part is an efficient top down design workflow. You use
common modeling commands to create a new body in the context of other bodies. Use
sketch-based modeling commands like Extrude, Revolve, Loft, Sweep, and Coil to
create a new body by selecting the New Solid option in the dialog box. See Figure 8.
Make Components
After you created your Solid Multi-Body part, you can start creating the assembly
from the part file (skeleton). New solids will be selected and will become new parts
as individual IPT files. These files are automatically inserted into a new assembly.
Figure 9 – Solid Multi-Body part
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Workflow: Make Components from Solid Multi-Body part
1. On the ribbon, click Manage tab | Layout panel | Make Components.
In the Make Components: Selection dialog box, you select the solid bodies to
derive in the model browser or onscreen selection.
Target assembly name – by default, is the same name as the layout part. It’s
good practice to leave it that way. It will be a lot easier to find, and the
relationships will be more apparent. Otherwise, use your file naming system.
Template - Select or browse to the assembly template from which the new
assembly is created.
Target assembly location - browse to the location where the new assembly is
saved. Use to select an assembly that exists, if appropriate.
Figure 10 – Make Components: Selection dialog box
1. Click Next will allow you to edit the Component Names, Template for the
component, BOM Structure, individual File Location or include Parameter.
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Figure 11 – Make Components: Bodies
2. Select OK. This will create an assembly with all the bodies as new components
grounded together at the origin of the file. Save the assembly. (See Figure 9b)
Watch Converting Bodies to Components video for more information.
Post - Make Component considerations
You will need to consider assigning materials to the new parts since derived parts
do not propagate material settings. We will use the Bill of Materials command to
update properties such as Material, Mass, Thumbnail, and other relevant iProperty
metadata.
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Figure 12 – Bill of Materials
To assign material to a part, you will need to add the Material column to the Bill of
Materials table. Follow the arrows as shown in Figure 12. Drag the Material and drop
in between the column headers of the Bill of Materials table. Do the same steps for
other property metadata.
6. Summary
Begin with the end mind. You should be able to picture the finished product before
you start using Inventor. Use this requirement to fully utilize the Skeleton Modeling
process.
Keep it simple. Make your sketches simple and clean. Create relevant sketch names
for different components. Drive the sketch dimensions using parameters created from
an Excel spreadsheet.
Derived to Make Components. Now you know the 2 methods of modeling an
assembly use it. You can use either or both of the 2 methods. Use the GEA CAD Tools
Move to Origin to assemble all components with just a click.
If you have any questions or ideas that will help to be more productive in using this
workflow, please email us at DAWN@gea.com. We would love to hear your feedback in
using this manual. Thank you! 
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