Inventor – Assembly Constraint Naming

Management of features and components in Inventor is kind interesting.  In AutoCAD, the technician is free to create things in almost any way.  A great deal of management is required to be efficient.  I recall using Inventor for the first time.  It was such a relief, because Inventor automatically took care of entity management through styles.  Features however are a different story.

Naming features such as constraints is one option available to help reduce the confusion in Inventor.  If you don’t rename constraints, you can end up with spaghetti.  Waiting until you have a troubleshooting session to rename the Assembly Constraints will result in a disaster, because you will have numerous Constraints all named similarly.

Design Accelerators compound the issue because they autonomously create features at once, without consulting the user for names.  When you get done with a few gears, you have a mess.

In this example I was troubleshooting why my actuator was not moving in the assembly when the motor motion was applied.  When sorting constraints out, I recommend 3 things:

Changing to Modeling View

Changing the view will group all the constraints into 1 region, assembled into 1 feature instead of broken into pairs over the 2 respective constrained components.  This allows us to see them in a simple collection.

Rename the Assembly Constraints

Renaming the Constraints as you go is quite important.  After creating 2 sets of gears and a shaft, I have about 18 constraints named Angle:2 and Mate:5.

So I like to give them names that include:  The 2 components that are being constrained; The purpose of the constraint; possibly the nature of the constraint as well.

In this example I had an overlapping constraint, but could not see it until I had changed to Modeling view and finished renaming everything.  I pick each object, and Inventor highlights the planar faces and features that are associated in the Constraint, which allows the user to get a feel for what is going on.

I renamed this angular constraint to WormToSpurGearLock, so I would see the 2 Gears involved (Worm and Spur gears), and the purpose was to lock their rotations together.  In another I used MotorShaft-Drive so that I could find the Drive components quickly and distinguish them from the others.

Isolation

If I wasn’t sure what was constrained, which is often the issue, we can Isolate the pair.  This way it is quite easy to see how and what is being constrained.

 

Thoughts

Once the naming was complete, it did not take long to read each one, and check off the list of what was expected between each component. Eventually I found where I had included an angle control on the shaft that would not allow the actuator to turn.

Naming your Constraints as you complete procedures, whether it be manual assembly, or Design Accelerators is a good habit to get into.  In his example I just needed to proof out a solution, but inevitably wanted to keep it.  Taking the small amount of time to name the constraints as you go will really pay off in the future.

Inventor – Weld Gap nominal parameter

I’d like to see a way to get the Frame Generator tools to access the parameters.  I am a top down kind of guy, and like using extrusions and dependent sketches for my frame skeletons.  I derive almost everything to keep all my parameters centrally located. 

The design I am currently engaged in was started without some specs, and after receiving them I find that he builder does not want any weld gapping.  So I have to run through every weld and remove the gaps.

It would be nice to set the gaps a local parameter that is factored from a derived parameter, like ‘NomWeldGap = MatThickness * NomWeldGapFactorl’ or something similar.  This way I can change the NomWeldGapFactor in the skeleton, and all the gap would alter in relation to their individual material thicknesses. 

Publish Content for Bolted Connection Part 4

Content Center Family Editing

We need to change some settings in the Content Center Family just written.  Navigate through he Content Center Editor to the new Family.  Right Click, and select the Family Table option.  The family parameters dialog will appear. 

The following are examples that I used, however you will undoubtedly have differences and variations at your company that need to be adopted.

 

Publish Content for Bolted Connection Part 3

Content Center Category Review

We need do some snooping.  We need to know where we are publishing the content.  The Countersunk Bolts Category is our target.  It would be ideal to publish our content to the sub category of ‘Wood Screws’ but alas, this cannot be.  You see the Design Accelerator has a limitation (I’ve heard this before….limitations), in that it will not use content below a certain sub-category.

 

The Bolted Connection Generator will only read from the Categories:

• Countersunk
• Hex Head
• Hex Head – Flanged
• Round Head
• Set Screws

We cannot file our content appropriately and get the desired outcome.  Once again we have to hack up a beautiful landscape, but the benefits are worth it. (I am still convinced that I will find the directing XML, and modify the strings to go deeper.)

The publishing process will take our part, and store it with the iPart members as members of the new Content Center family.  The family will take on the properties of the parent category, and we need to know about that criteria.  We have to direct the publishing to map the iPart parameters to the appropriate category fields. 

Let’s take a look at the Category Properties for the Fasteners->Bolts->Countersunk sub-category.  You should see the list of data contained in the category, that gets passed down to the individual families contained therein.  It’s a form of inheritance.  Notice the Mapping field, and the Optional and Required options.  The required settings are brought in from the parent category, and cannot be left out of the mapping.

Publish Content for Bolted Connection Part 2

Back to Part 1

iPart

iParts are method of creating Library Contents for similar parts. When you create an iPart, a table is placed in the part, that will contain the individual members of the library.  These members are contained in rows of the table, with the key differences edited for each member.

The table contains various fields that represent the parameters that shape the iPart members.  The iPart members can have identical values as needed, with the exception of 2 fields.  The Part Number and Member name.  A lot of care should be taken in planning the Part Number and Member names, as the future file name of library contents is tied to the Member Name, and the Part Number gets fed into the BOM.  However, the Content Center Editor can apply variables from the table to concatenate a Part Number automatically, which we WILL do later.  For now, we will prepare the table in the following fashion.

Under the Tools Menu, select Create iPart.

The iPart Author dialog will appear, revealing the structure and rows that will appear in the iPart table.  Currently there is only 1 row in the iPart table, seen at the bottom of the dialog. This row is fed from the current parameters contained in the part.

 

Publish Content for Bolted Connection Part 1

Read the Introduction

The first thing that needs to be completed is kind of the core to this process.

Thread.xls

Normally we would begin in an assembly file, but for this exercise we need to go mess around with Autodesk’s artwork.  We need to edit the Thread.xls file.  You see, the Bolted Connection Generator as well as everything else in Inventor derives it’s threads from this file.  This file contains a beautiful collection of thread data, including Inch, Metric, and tapping threads.  Unfortunately the facts that bring us here today is that:

a) there is nothing available for ANSI/ASME B18.6.1 Wood screw threads; and

b) The Bolted Connection Generator only reads data from the first 3 thread tables in that file (ANSI Unified, ANSI Metric, ISO Metric).

What we need to do is to add a new row for the B18.6.1 thread for a #6 screw.  The new row needs to be added in the ANSI Unified Screw Threads Table.  Why? Because if we don’t, the Bolted Connection Generator will not use it. I know this is in bad taste, but it will get the job done.  I have no doubt that the table restrictions in the design generator is coded in XML, and that I will eventually find and exploit it.  For now, this is the only way.

Navigate to the following VISTA path:

C:\Users\Public\Documents\Autodesk\Inventor 2009\Design Data\Thread.xls.

Open this file with Excel and navigate to the ‘ANSI Unified Screw Threads’ Tab.  Select the first #6 thread entry row header, Right click and select Insert.  You should see an empty row appear. Add the data from the highlighted row in the table shown below.

Close and save the file.  Let’s start the next step by opening a new Inventor assembly.

Publish Content for Bolted Connection

Everyone knows I love Design Accelerators, Content Center, User parameters, derived components…..Ok I just love Inventor.

The Bolted Connection Generator is a fabulous tool. It creates a filter criteria using diameters found in the selected thread type. It then uses that to filter the Content Center selection to create a list of fasteners.  The holes and recesses are created from geometry in the separate data.  The list of possibilities however, has some limitations.  I’d like to show you 1 way to get more productivity, working within the limitations. 

If I can get the job done with a Design Accelerator, then why would I want to prep everything without it?

This discussion is a workflow I performed recently to get some new fasteners into the Bolted Connection Generator.  Again, the theme has to do with wood, as I found a lot of people asking about wood, and little assistance was available. 

This workflow will take us through the following topics:

• Thread.xls
• Sample Part Modifications
• iPart
• Content Center Category Review
• Component Authoring
• Content Center Family Editing
• Bolted Connection Generator

Part 1 of Create Read/Write Content Center Library

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