IMAGINiT Manufacturing Solutions Blog

Inventor "Redefine (Work) Feature" Command

Recently I published an article on the Inventor "Redefine" command which was used to redefine the plane or face a feature sketch was created on.  This article is about another valuable tool found in both in the part and assembly environment.  In the title I placed "Work" to emphasis that the "Redefine Feature" command is used to change the location and orientation of any existing Inventor work feature in the model.  The power of this process becomes evident if a feature or a sketch is connected to the work feature being redefined.  In my model below, the side extrusion sketch has been created on a work plane which is parallel to the origin X-Z plane and tangent to the outer diameter of the model.

The extruded feature is modeled 180 degrees from the end keyway.  The design has changed and the feature needs to be at 90 degrees to the keyway on the front side.  Thinking back to the steps used to originally create the feature, you realize it will take quite a few steps to re-model it.  This situation is a perfect example to use the "Redefine Feature" command.  The theory is simple, since the feature sketch was placed on the created work plane, use the command to simply redefine the location of the work plane and the sketch and the extrusion will follow.  Any valid method can be used to create the redefined work plane, in this case the same method will be used except the origin Y-Z plane will be used as the reference plane.  Along with the selection of the outer diameter of the model the work plane will be redefined to a new position carrying the feature sketch along with it.

Right click on the sketch work plane and select the command "Redefine Feature".

At this point the extrusion feature will disappear but do not worry, it will return after the work plane has been redefined.  Select the origin Y-Z plane and the front outer diameter of the model.  The work plane appears and the extrusion moves to the new design location.  How is that for speed?

Occasional when using the "Redefine Feature" tool to redefine a work plane, the resulting work plane will develop with the "normal" side pointing to the model.  This will cause the existing extrusion to fail because the extrusion direction is pointing away from the main model.  There are two quick fixes for this condition, I will mention both so you can choose.  Below I have redefined the work plane to the back side of the model.  You will notice that the extrusion has failed and the light orange side of the work plane is toward the model.  I am right clicking on the edge of the work plane and selecting "Flip 
Normal" from the menu.  This will correct the extrusion.

The other solution is to select the extrusion feature and right click.  From the right click menu select "Edit Feature" and simply reverse the direction of the extrusion.  Remember there are always more than one way to do anything in Inventor!

I must warn you that if the work plane has been used to create or define other model features or work features, the process can get complicated.  Plan well and your Inventor models will be easy to use the "Redefine Feature" command to make changes.  Do not forget, this command works on work axis and work points as well.

Custom Tube & Pipe Styles: Creating a Custom Tube & Pipe Style

Thus far in this series on creating an Inventor Tube and Pipe style I have looked at the steps required to prepare and publish a model for the Tube and Pipe environment. Before we can successfully use a customized component in a piping run, the steps in part one to three of this series must be followed to create connection intelligence. There are four steps in all to create a custom Tube & Pipe style:

1. Modelling a custom part (conduits and/or fittings)
2. Authoring a part as a Tube & Pipe component
3. Publishing a part to the Content Center
4. Creating the custom Tube & Pipe style

In this post I will run through the final step in this series and create a tube and pipe style using the same custom conduit I authored in my previous post. With all of the work authoring and publishing a part done, this final step in the process is where the part is actually specified for use.

If you are in a multi-user environment and you would like your tube and pipe styles to be shared with all users in your team you first need to make sure that everyone’s workstation is using the design data folder located on a network share. Even though the content center is usually centralized through Vault, or by moving the content databases to a network share, the tube and pipe environment makes use of another resource within the design data folder to manage piping styles. You can set the design data location in either the project file or Inventor’s application options.

Note: The project location will always override the application options if set.

To create a new tube and pipe style in the design data folder open the piping runs.iam file located in ..\Design Data\Tube & Pipe\en-US\

The piping runs.iam file is the template used to create any new tube and pipe assembly and contains all of your piping run styles. Any style saved in piping runs.iam file will be copied into new tube and pipe model assemblies.

With piping runs.iam open, Inventor automatically starts the Tube and Pipe environment. Select the Tube and Pipe Styles button to create a new piping style.

Once in the Tube & Pipe Styles dialog box you can edit existing styles and create new piping styles, either from scratch or by copying an existing style. For the example I used in this series I will need to create a new style in the Tubing with Bends category.

Clicking New activates the general tab for the new style. First enter a descriptive name for the style. This is the name that will be displayed in the list to the left and in the drop-down list when selecting a style for a piping run. For my purposes I’ll name this ASTM A 269 – Tube with 2 Parflanged Ends. The Category can be left blank.

The next area is where I will pick the authored components from the content center to use in this style. Double-clicking the Pipe row brings up the Library Browser where we can select the applicable tube to use in the new style.

Only Tube and Pipe authored parts in the content center will be listed here. In my case I renamed the published family (in the content center) to match the style name I entered above so I’ll find the ASTM A 269 tube and select the 3/8 inch diameter size from the library then click OK.

 

Note: With a new style you can select any appropriate size and standard component to start the style off. Once you have picked the first part (or you are editing an existing style) and added it to your style you will only be able to pick subsequent parts like elbows, couplings, etc. that have the exact same nominal diameter. Multiple diameters require a style for each diameter of tube or pipe that you wish to use in a piping route.

Below we see that the pipe row has been populated and the icon to the left of the table shows a green check indicating the component is in use. Secondary components, such as couplings in this case, are typically optional to the style.

Double-click on the Coupling row to select a library component for use in the style for couplings.

Note: You cannot add more components into the style list than what the editor allows. Depending on the style type; tube, hose or pipe and whether there is a slope added, there will be some options for other components but in general this list is fixed.

The second component in the style – you will notice – is automatically filtered by nominal diameter. If a family of components does not have a part with the diameter used then you will not see a line listed. In my case above I do not have an appropriate coupling so I will simply Cancel and leave the coupling empty.

Back in the style dialog box the diameter area should be prefilled based on the pipe selected. These should be left at their displayed values. You can also then change the component appearance setting if desired.

On the Rules tab there are a few more required fields before my style can be finalized.

Enter the Minimum, Maximum and Increment lengths as well as your default bend radius since this style is for tube and contains no elbows. My case above I have entered the values in millimeters. When finished hit Save to create the style.

In the left hand pane you should see the new style in the list under the tubing category. Save the piping runs.iam assembly and try creating a run using the new style in an another assembly file.

Note: when upgrading your Inventor software don’t forget to migrate this assembly and any applicable content libraries forward to your new installation.

-DP

 

Inventor "Redefine" Sketch Command

Inventor designers, one time or another, will place a sketched feature on the wrong plane or face of an Inventor part.  This may happen accidentally or maybe you received the wrong information, it does not matter.  You are looking for a quick method to "Redefine" the feature to the correct location.  In the part model below, the cylindrically feature should have been sketched on the origin X-Z plane instead of the current origin X-Y plane so it projects out of the top and bottom of the part.

The Inventor "Redefine" sketch command is a quick answer for this situation.  Locate the cylindrically feature's consumed sketch in the browser.  Right click on the sketch and select the "Redefine" command.

At this point all or some of the model features will disappear probably making you wonder if you want to proceed.  This in normal, take a deep breath and move ahead.  Looking at the lower left corner of the Inventor application, you will see the program is asking your to "Select work plane or planar face to redefine sketch".  Always look in this location for instructions in all Inventor commands and routines.  Expand the origin folder and select the X-Z plane and voila, the feature moves to the correct location!

You are probably patting your self on the back at this point and ready to move on, but you have one more step you must do.  When you redefined the sketch to the new origin plane, it lost some or all of its sketch constrains, you need to put them back to keep a valid design.  Edit the sketch and add any needed sketch constraints. In my example, all I need is a coincident constrain between the circle center and the part origin center point.  If you keep your sketches simple when you model, this step is a breeze.

Once it is fully constrained, finish the sketch and then pat yourself on the back for a job well done.  One more thing, this process will be a little more difficult if this sketch or feature has been used in the creation of another sketch or feature.  Plan accordingly.

Recovering an Inventor Part or Assembly File

It happens to everyone once in awhile, you modify an Inventor part or assembly save it and then realize you actually need the previous version and wish there was a way to recover it.  If you are using the Autodesk Vault, you can do this very easily since it creates and retains a version of every file checked into the Vault.  But what if your company is not using the Autodesk Vault, is there a way to do this in Inventor?  Yes and it is an easy process also.

The configuration of Inventor, to retain previous versions, starts in the Inventor Project file.  You company should only be using one project file for all jobs so this is a quick operation.  Open up Inventor and make sure no files are open.  Navigate to the Inventor project file by selecting the "Projects" icon as shown below.

In the Project dialog box, your current project file should already be selected.  Look at the area shown by the top read box and make sure it does not say the file is read only.  If it is, navigate to the project file location on your hard drive and remove the read only property.  Next expand the "Options" entry and note the number setting for the "Old Versions To Keep On Save".  This number represents the number of "Old Version" files Inventor will keep for each model when you save.

It is not recommended to change this value to "-1" since that will keep all old versions and will lead to a rather large "OldVersions" folder taking up a lot of unnecessary hard drive space.  It is set to "1" during installation which is usually adequate for most companies.  Set it to a higher value if you see fit.  If you made changes "Save" the project file and close it.

Now I would like to demonstrate how this feature works.  I have opened an Inventor part and decided to remove two mounting holes in the part because I was told they were not needed.  I then saved the model file and thought I am finished.

A couple of days pass and I am informed these two holes should not have been removed.  I puzzle over how I can recover them not remembering the placement or the size.  Then I remember I have configured Inventor to keep old versions.  Using the "Open" command, I look in the folder that contains the model file and notice the "OldVersions" folder.

Inside the "OldVersions" folder, I find my file by the same name, with a number appended to it.  This number has been added by Inventor during the save operation to make sure the file name is unique.  

  I open the file and a message box is presented.  The options are self-explanatory, I want the "Restore old version to current version" to recover my part with the mounting holes.  Select "OK" to open the restored file.

  
Make sure you save your model once opened to restore your file to the regular folder structure to complete the process.  If you are doing a "Pack and Go" of a model, it is advisable to search the folder structure for all the "OldVersions" folders and delete them to make your pack and go file size is as small as possible.

So next time your make a change that needs to be recovered, Inventor old versions are a snap to use as long as you know where to look for them and how to use the recover feature.

Sharing Inventor Model Parameters Between Parts

There are three main methods for sharing Inventor model parameters between parts.  You can use the "Derive" command to import parameters from another part.  Using this method you can share both "Model and User Parameters.

The second method is to "Link Parameters" between models by using the "Link" command in the "Parameters" dialog box.

Both of these methods create a shared link between the original model parameters and the new model.  If changes are made to the original shared parameter, the change occurs in both models.  This behavior can be suppressed or broken when using derived parameters.  If the derived link in broken, the shared parameters automatically become "User Parameters" in the derived part. 

If the "Linked" parameter model folder is deleted from a parameter table, only the linked parameters that have been used in the new model are retained and changed into "User Parameters", the remainder will be deleted.

The third method is a little different.  The method is to import parameters, using the "Import from XML" command, using previously exported command from another model using the "Export to XML" command.  Both of these command are found in the expanded menu under the "Parameters" located on the "Manage" tab.

Using this method you are simply making a copy of the model parameters from one model to another.  No linking of parameters occurs.  This method will export and then import both "Model Parameters" and "User Parameters".  This method has the extra ability to export and import "Text" and "True/False" user parameters.  The "Text" user parameter can even contain a "Multi-Value" list.

This method has another advantage in that the parameters may be imported from as many models as required.  This has one restriction, the parameter name must not already exist in the model being imported into.  The import process will import all the other parameters, give a warning that the offending parameter will not imported and skip it.

There is may be one concern about using this method and that is you cannot control which parameters you import which is possible with the other two methods.  This should not be a concern because the model parameters table has a "Purge Unused" command that can be used to discard all imported parameters which were not used in the new model.  This command was added in Inventor 2015.

I hope you see the power of the third method especially when you do not want to share linked parameters between models.