IMAGINiT Manufacturing Solutions Blog

Vault File Lifecycle Management - Release Biased

If your company uses Vault Workgroup or Professional for File Lifecycle Management, you may have noticed an icon on the Preview panel that looks like the follow screen shot.  When you select it the arrow either points up or down and you see something about "Non-Released Biased" or "Released Biased.  You may wonder what these conditions mean or do with your data selection.

  To explain these conditions, we will use an small Inventor assembly.  You will notice that the assembly and its associated parts are in a "Released" lifecycle state.  The revision scheme being used in alphabetic. 

Some time passes and it is decided that a Word document needs to be attached to the assembly that contains supplies needed for shipment.  The Word document is already released and has a revision level of "2".  By category all Word documents use a numeric revision scheme.  The Inventor assembly model lifecycle state is changed to "Work in Progress" and the revision level is bumped to "B" then the Word document is attached.

The assembly state is returned to "Released.  Looking at the "Uses" tab we see the attachment on the "Latest Released" of the assembly.  Notice the icon is pointing down which indicated a Non-Released Biased" condition.

 
If the revision level "A" is selected, the icon changes to a "Released Biased" and you will notice the attachment of the Word document is missing.  The Vault is remembering that you did not have any attachments to the assembly when it was at revision "A".

  Some time has passed and the Word document goes through a revision cycle to add some extra shipping supplies needed for another assembly.  When the Word document is changed back to "Work in Progress" the revision is bumped to "3".  You worry this may create a problem because this will change the shipping supplies document attached to the previous assembly but the Vault takes care of this issue.  While the Word document is in a "Work in Progress" state, you click the icon to change it to "Released Biased" and the correct version of the attached document is display for the latest version of the assembly.  Revision "2" was the version of the Word document released with the latest released version of the assembly.

If the "Non-Released Bias" option is selected, the attached document is version "3" for the latest release assembly.

  Once the Word document is re-released, the latest revision of the assembly uses the current document version.  If you select a previous release of assembly you will see the correct document revision assigned.  Below are two screen shots showing these two selections.

This idea holds true for the assembly parts as well.  Time as passed and some of the parts have been revised at different times.  Below are two screen shots showing the latest release state of the assembly and a previous revision state.  Compare the revision levels of the parts and you will see that the Vault has maintained the correct revisions per assembly revision.

   
This ability of the Vault to remember which revision states for parts and attachments according to the revision level of the assembly is far more trustworthy than our own memory.  As time passes we can still return to the Vault, select the desired assembly revision level and then use Pack and Go to retrieve all the parts and attachments that were current at that time.

There will be times when you would like to change the revision level of an assembly attachment to a different level.  This process starts by changing the assembly to a "Work in Progress" state then while the assembly is selected, pick the "Attachments" command.  In the dialog box simply select the desired attachment revision to be hooked the assembly.  You could even return to a previous revision of the attachment.  Once selected, pick "OK" and finally change the assembly lifecycle back to "Released".

  

Vault Batch Plotting all Drawings for an Assembly

I published an article the other day on how to batch plot all the drawings related to an assembly.  A short time later a reader pointed out to me that there was a much easier method than the one I suggested.  I am editing my article to reflect his method.  This method also only applies to Vault Workgroup and Vault Professional since they are the only Vault packages that contain the batch plotting utility.  I left the old article in this post just for the record, it is marked as such.

Without any files selected in the main panel, select the batch plotting icon or the command from the File menu.

Select the "Add" dropdown menu and select "Add Related File Sheets". 

Browse in to the assembly file you want plot the related drawing files.  Select the assembly and press "Open" to continue.  The Vault will be searched and all the drawing files will be placed in the plot manager dialog.

Select the entries, configure the plotting device and settings and you are done.  This is by far a much better method that my earlier article outlined.  I wish to thank Brendan Henderson for writing me and suggesting this method.

 

Original Article

The ability to select an Inventor assembly in the Vault and then select the "Uses" tab on the Preview panel creates a list of all the sub-assemblies and parts used.  Most Vault users are disappointed it will not also show all the related IDWs or DWGs.  If the Vault will not provide this functionality, then it is safe to say it will not allow you to find all the drawings related to a selected assembly and batch plot them.  This article will outline the process to do just this operation.  It is not real pretty but it gets the job done and once you do it a couple of times, it is pretty fast.  The full process of batch plotting process in unavailable in Vault Basic but the sorting of all the drawings related to an assembly is.

The first step is to create a scratch folder in the Vault.  Name it something that reminds you of the folder's purpose.  I created one called "DWF Plotting Folder".  Use the "Go to Working Folder" command to create the same folder in your local workspace.

  
Next, select the assembly file you wish to find all the related drawing files.  Select "Pack and Go" from the File menu.

Configure Pack and Go according to the screen shot below.  This will find all the DWF or DWFx files for the assembly, sub-assemblies and drawings of the selected assembly.  I am assuming at this point that your Vault is using visualization files and all are present and available. 

Select "OK" to continue and then select the temporary plotting folder created earlier in your local workspace to receive the files.  You probably will receive a warning about the visualization files being out of date, select "Yes" to continue.  You will now have all the DWF files in the local workspace folder.  Now return to the Vault Client and right click on your plotting folder in the navigation panel and select "Add Files". 

You will want to exclude the old versions folder and the Inventor IPJ file before you place the files in the Vault.  Select "OK" to finish.

In the Vault select the "Find" command.  You are going to create a saved search that will sort out all of the DWFs except the drawing files.  Configure the search as shown below making sure to replace my search folder with yours.  If you use DWG for your Inventor drawings, substitute dwg for idw in the search string.  Save the search so you can use it over and over.

  After you execute the search, all the files in your temporary plotting folder will be the drawing files ready to be batch plotted.  Select all of the files and select the batch plotting icon to begin. 

 
Since batch plotting is not in Vault Basic, you will have to use some other plotting method but at least you have all the drawing files from your assembly in one place.  I batch plotted my drawings to PDF files using the Vault batch plotting routine and Adobe.

Last, delete all files in your plotting folder both in the Vault and in your Vault workspace so you are ready to go with the next assembly.  This process seems long but it is has one big advantage, it will find all assembly drawings not matter where they are in the Vault and allow you to print them as a group.

 

Improvements in the Inventor 2017 "Import" Command

This article will highlight some of the the improvements in the Inventor "Import" command when used to import an AutoCAD 2D drawings.  This command is a part of the "AnyCAD" functionality which was first seen in Inventor 2016.  The command functions in basically the same way but new functionality has been added in Inventor 2017 making the process easier and more useful.

One of the main features, of using the command with AutoCAD drawings that has not changed, is the adaptive linking between the Inventor part and the AutoCAD drawing.  This linking may be suppressed or broken at anytime.

The first improvement is in the "Translation" command.  This function is in both versions and allows the re-positioning of the imported AutoCAD drawing in relation to the part origin or an existing part model.  An improvement has been added to the "Location" sub-function within the command.  A drop down box has been added with an additional function "Location to Origin".

This allows the moving of the AutoCAD drawing views to the origin of the model or model key points in one step.  In Inventor 2016 this process was accomplished in two steps.  Simply select the "Locate to Origin" sub-command, click on the green dot on the origin icon and then select the point on the AutoCAD drawing you want to move.  the AutoCAD drawing will instantly move to the origin.

The command "Project DWG Geometry" is the same as in Inventor 2016 and allows you to project single, connected and block geometry into your sketch.  All projections establish the adaptive link back to the original AutoCAD drawing.  The next big improvement is the change in the method of adding another instance of the base AutoCAD drawing.  This is needed when you are creating features on different planes or model surfaces.  In Inventor 2016 you would have to use the "Import" command to bring in the AutoCAD drawing for the second time.  In Inventor 2017, right click on the first instance of the AutoCAD drawing and choose "Add Instance".  It request the plane or surface you want to place the instance and then request the origin point which in identical to Inventor 2016.  Using the new "Locate to Origin" sub-command makes for easy alignment of the drawing to the select origin.  The availability of on screen rotational drag are the same.

The "Visibility" and "Layer Visibility" are a part of both Inventor versions but Inventor 2017 allows the ability to "Crop" the under lying AutoCAD drawing in the model.  This has uses in the model but the main purpose of this command is to allow special views in the Inventor model drawing.

Once the drawing of the model has been created, you discover another new feature, the ability to "Include" any instances of the AutoCAD drawing into the Inventor drawing view.  Used with the "Crop" and the "Layer Visibility" commands back in the model, you can get some interesting drawings very quickly.

For example, by including the first AutoCAD drawing instance, all of the drawing views are automatically dimensioned.  These dimensions were in the AutoCAD drawing  and since the drawing instance in included, they appear.  You can get different results by manipulating "Layer Visibility" and the "Include" command.

Once the AutoCAD drawing is included in the view, a "Visibility" option is added to the right click menu.

I hope you will take a look at this new functionality in Inventor 2017 and find out just how easy it is to use AutoCAD drawings in your designs.  One final note, please do not forget that the AutoCAD drawing is adaptively attached.  Unless this feature is required, it may be a good idea to either suppress or break the link. 

 

Changing a Pattern in an Inventor Solid

Whenever you import a third-party part model into Inventor, most of the time you end up with a featureless solid.  Inventor over the years has improved the tools available to edit these solids either directly or in the creation of features from solid entities.  Below is a SolidWorks part imported into Inventor 2016 using the AnyCAD application.  The model is feature entity rich, but once imported it is a dumb solid to Inventor.

Among the solid editing tools are ones that will move, rotate, size, lengthen, delete, etc. the entities of the solid model.  The focus of this article is to present a method of accomplishing the modification of an array within a solid.  It is not a direct command but a combination of a few.  The process can save a lot of time and effort.  If you desired to change the patterned hole count around the center of the above solid, you would find out quickly that the pattern feature tool does not work since there are no (Inventor) features in the model.  The most effective way to do this part is to simply delete the existing pattern add a new hole, chamfer it and then pattern to the desired count.  But what if you had a solid where the pattern was made from a cutout shape not as easily duplicated.  A example of this is shown below.  Sure you could use the same method outline above but read on, maybe the process below will be easier.

The first step is to create surfaces from one of the triangular cutouts in the pattern.  I will select the one facing one side of the plate.  Creating surfaces from existing surfaces is quickly done using the "Copy Object" command located on the 3D Model Tab under the Modify panel.

Starting the command, I first make sure that I will be selecting faces not solids and that I will either be creating surfaces or composite surfaces, either one will work.

After selecting the three inside faces of the triangular cutout, select "OK" to finish.  The browser shows the new composite (group of surfaces).

The next step is to close off each end of the triangular cutout with a boundary patch.  The "Patch" command is found under the 3D Model tab, on the Surfaces panel.

To create the patch, select the three edges of the cutout and select "Apply".  Repeat the process on the opposite side.  You now have the cutout area completely surrounded with surfaces.

The next step is to create an Inventor Solid Body inside these surfaces using the "Sculpt" command which is located right below the "Patch" command shown above.  Select the option to create a "New Solid" in the dialog box and then select the three surface features in the browser. 

After selecting "OK" to finish, you will notice that a new Solid Body has been added to the model.  Select it to confirm it is the triangular plug in the model.

The next step is to remove all the existing triangular cutouts from the original model, including the one used to make the new solid body.  The Inventor tool used for this is the "Direct" command located on the 3D Model tab on the Modify panel.

Select the "Direct" function and select all the triangular cutouts in the model.  You can use a "Window" selection method (left to right), maybe two, to make this job very quick.  Select the "+" command to finish the task.

   What you have left is the original solid body you imported and the triangular solid body that your created earlier.  The next step it to remove the triangular solid body to create the triangular hole.  The "Combine" tool, located on the 3D Model tab, Modify panel (see above) makes this an easy task.  Select the original part as the "Base" and the triangular body as the "Toolbody" then "Cut" for the operation.  Select "OK" to finish.

The last step is to pattern the feature (Combine1) to the count you desire.  In my example, the array originally had 6 instances, I needed 12.

The process may seem long when you read and executed it for the first time but with practice, it will become a minute or two process.  Also, think of the time you have saved not having to model the feature and possibly getting a dimension error or worse.

 

Adding Inventor iProperties from the Drawing

There are many ways to enter Inventor iProperties into your models and drawings and in this article, I want to mention one more.  This method is an excellent way of entering iProperties that populate the drawing title block, drawing border or sketch block(s) from the drawing view.  You may have noticed the "Edit Field Text" command under the title block entry in the drawing browser.  This command appears in two other places allowing the direct entry of iProperty values in the drawing border and sketch blocks.  It is rare that a company's drawing border has iProperty entries but it can be a powerful tool.

Selecting this tool will open up the Edit Property Fields dialog box.  It will display all the Inventor iProperties which exist in drawing section selected.  In the graphic below, I selected the drawing title block which contains all the iProperty types.

Most everyone is probably familiar with "Prompted Entry" drawing iProperties.  These are the ones presented to you every time you start a new drawing (if they exist).  A little side note here, if you are using or planning to use the Autodesk Vault and would like to index an Inventor iProperty into a Vault user defined property, do not use prompted entry as a method of iProperty entry.  Vault will not recognize prompted entries.

Most everyone will use a mixture of the other types of iProperties types to populate the title block.  Some of the types are not editable such as "Sheet Properties" which are system iProperties.  Others you know you can edit from either the model or the drawing but they are grayed out in the dialog box.  The secret to editing these is the icon located in the top right corner of the dialog box. 

  Highlight the iProperty you wish to edit, select this icon and it will open the iProperty dialog box containing the selected iProperty.  For example, if I select "Description" and press the icon, it will open the part iProperty dialog box.  One shortcoming of the process is it will not open the Project tab where the Description iProperty is located, I had to do that myself.

The following Edit Property Fields dialog shows the available iProperty types available when I "Edit Field Text" of a sketch symbol.  Notice the sketch symbol only contains two types of iProperities.

One word of caution before I end.  Most iProperty values in the drawing title block, border or sketch symbol will update immediately after leaving the Edit Property Fields dialog box but not all.  This can be easily remedied by selecting another open file tab and then returning to the drawing.  You also can just save and close the drawing and the next time it is opened it will show the updated value.

The next time you need a quick iProperty entry from the drawing view, consider using the "Edit Field Text" command.