IMAGINiT Manufacturing Solutions Blog

Simulation for the Modern Manufaturer webcast

This past Wednesday IMAGINiT conducted a webcast focusing on simulation tools.  John Twerdok from Autodesk discussed trends that are occurring in simulation tools and engineering.  Garret Rausch, an engineering manager with Menges Roller, discussed how simulation tools have benefitted his company.  And Carl Smith discussed how to review your process to find the areas that would benefit most from this technology.

You can view the webcast recording here on our customer portal.  You will need to sign into the portal to view the recording. If you have not signed up for our portal yet, it is free and only takes a few minutes.

Adding Inventor Part Sketches to Drawings

From time to time you will have an Inventor part which either entirely consists of parametric sketches or will contain both 3D model features and sketches.  The process of placing the sketch entities on the drawing will vary slightly between the two situations.

If your part contains only sketch entities, when you place the part model on a drawing view the sketch entities show up immediately.  If you place a part model consisting of both 3D model features and sketch entities, the sketch entities will not show up automatically.  You have to add them to the view by right clicking on the part, below the view, and select "Get Model Sketches".

In both cases, once model sketches are included in the drawing view, you cannot uncheck the "Get Model Sketches" option.
If you wish to remove a particular sketch entirely from the drawing view, expand the part, right click on the desired sketch and then choose "Include" to toggle it off and on.  You can also select "Visibility" if you desire.


In the above screen shot, notice there is a selection to toggle sketch text on or off in the drawing view.

The last thing I want to mention is how you can apply sketch properties to the model sketch and they can be shared to the drawing view.  To change the properties of model sketch entities, select them, right click and select "Properties" from the context menu.  Change the styles as desired.

If the drawing view, containing the model sketch entities, already exists, you will have to right click on the changed model sketch and choose "Reapply Model Properties" from the context menu.

Of course, sketches in drawing views accept all annotations Inventor has to offer.

The next time you need a quick 2D drawing and you really do not want to switch to AutoCAD, sketch it up in Inventor.  One of the side benefits is the sketch will be parametric.

Autodesk Vault and Revisions - Part 1

I spend a large part of my day talking to people about data management in general, and Autodesk Vault in particular. One frequently asked question is “How do the revisions work in Vault?”  There is a lot wrapped up in that question.  A lot of times what clients are actually asking me is, “How can I protect my designs?” or “How can I ensure that the shop is using the correct file?” This post is the first in a series that will attempt to answer those questions.

Understanding file versioning

Before I discuss revisions, I have to review the concept of file version. Vault Basic, the version of Vault that is part of the Autodesk Design Suites, deals only with file versions.  A file version is a copy of a file that is created every time a file is checked into the Vault.

Every time?

Yes, every time.  That means that if you check a file in and out five times in a day, you will have five versions of the file.  Vault does not care if the file has been changed at all, it simply records each check in as new version of the file and maintains a copy of the old version the file store.  It is a very similar idea to the “Old Versions” folder created by Inventor. 

Versions also get created when certain Vault functions are used.  For example, renaming a file or editing the properties of a file will create new version as well.  The image below shows the version history of a particular file.

In this case, Version 1 was created when the file was initially added to the Vault.  Version 2 was created when the file category was changed.  Version 3 was created by checking the file out and then checking it back in, and version 4 was created as the result of editing the file properties in Vault.

With all of these versions of the same file in Vault, the question is often asked, “Which version do I get when I check a file out of Vault?”  The answer is simple: the most recent one.  This is known the leading version.  When a file is checked out of Vault, Vault checks to see what the leading version is of that file, and that is the one that gets checked out for editing.

Versions work very well for capturing the “work in progress” changes of a design file.  What they do not work well for is capturing specific design milestones. 

A new version is created every time Vault or Inventor changes the file, so this makes it dangerous to say that “Version 6 of this file has been released to manufacturing.”  If someone checks out that file, or changes its properties, that file is now version 7. 

To effectively mark milestone or release points, there must be a way to lock down the file so that no changes can be made to it. Next week I will review the tools that Vault uses to do that, Lifecycle States and Revisions.  But until then, I am curious: does your company use Vault today?  And do you track your file versions?

 

Cfunk

Creating Reference Geometry During an Inventor Sketch

There are three basic methods of creating reference geometry from existing edges and points when creating a new sketch in Inventor.  We will make an assumption here just to be clear, all the existing edges and points are on the same plane as the new sketch.  The first method is to use the "Project Geometry" command and either select the desired edges or select somewhere on the sketch surface to project all edges and points at once.  This method assumes that the "Autoproject edges for sketch creation and edit" is turned off in the Application Options on the Sketch tab.

The second way is to select the option shown above so all edges and points, that are on the same plane as the new sketch, are projected into the new sketch automatically.  This is the method a vast majority of users follow.  The problem with this method is that sometimes you just do not want all of the reference geometry that has been created so you waste time deleting it.

The third option is the one I want to talk about in this blog.  It is sort of a hybrid of the two earlier methods.  The setting allows for automatic creation of reference geometry by passing your cursor over existing edges and points, while sketching, and only retains the reference edges you actually used during the sketch.  The setting to turn it on is in your "Tools" "Application Options" "Sketch" tab and by placing a check mark in the box shown below.

Taking a look at an example, this is the final result of my sketch showing sketched lines and final reference geometry used.

During the sketch, I can hover over as many edges as I desire and they automatically appear as black projected lines and points.  If any of these are use as reference edges or points in my sketch they are retained and converted into reference geometry (green in my color scheme).  All other projected blacks lines that were not used are discarded.  Below is an screen shot showing all the black projected lines before the sketch was finished.


This process only works when you are sketching entities such as lines, splines, circles, rectangles, etc.  Of course at any time you can fall back to the "Project Geometry" tool to create reference geometry.

 

Replacing an Inventor Component with Similar but Different One

There are a number of ways to accomplish this task.  As you become more proficent in the use of Inventor, you will be interested in developing more efficient practices and methods for modeling and creating drawings.  This article will explore one of the assembly productivity tools, Save and Replace Component, as well as the drawing tool, Replace Model Reference, as one of these methods.

The design is a small machine which has a base plate with two mounting holes.  The design needs to be change to have four mounting holes, symetrical about the center of the plate.

With the assembly model open, select the "Save and Replace Component" productivity tool.  Select the base component and this tool will Save a copy, with a path and filename of your choice, and immediately replace the component in the assembly in the exact same position.  Best of all, all assembly constraints are maintained.

With a quick edit of the new component to mirror the existing mounting holes, you are finished with the edited assembly.  Of course you could save it out as a totally new assembly but that is not required for this particular task.

Next, you need to create a new drawing for the new component.  I am assuming that a drawing already exists for the old component with dimensions, notes and other annotation.  Open the drawing by right clicking  the new component, selecting "Component, Open Drawng".  You will need to browse and select the existing old component drawing.  Once the existing old component drawing is open, I would suggest that you immediately save it by the new component's name just to make sure you do not forget and save over the old drawing.

Navigate to the "Manage" tab and select the "Replace Model Reference"  command. 

In the Replace Model Reference dialog box, select the existing component from the list and then select the "Select New Model" icon.  Browse to the new component and select "Open".  Accept the warning with a "Yes" and your drawing will immediately update to reflect the new component.

The wonderful part is that all dimensions, notes, and other annotation were preserved.  All you are required to do is remove any sick dimensions and annotations for entities that were removed and add some new ones as needed.
 

The complete process will take you about half the time it takes to read this article once you have executed it a couple of times. 

 

Learn how to Produce More Innovative Products, Faster and Easier with Simulation at our Upcoming Webcast

Simulation for the Modern Manufacturer
Wednesday, February 25
2:00 PM - 3:00 PM Eastern Time

Join us at this online discussion and gain insight into the future direction of simulation and learn how the right simulation tools can get your products to market faster while increasing your ROI.

Key Takeaways

• Autodesk expert provides a glimpse into the future of simulation technology
• Menges Roller shares their experience with implementing a simulation solution
• IMAGINiT delivers best practices for leveraging an effective simulation solution

The presenters will be available for Q&A at the end of the session.

Registration is complimentary but required.

Learn More

How to Use Inventor Sketch Block Dimensions in Other Feature Sketches

Inventor sketch blocks are great ways to keep common sketches in your Inventor part template.  If you have common modeling features that require the same parametric sketch, Inventor sketch blocks can really speed the process of modeling.  An example of this can be found in the modeling of a seal groove in a flange fitting.  The fitting flange will change size and the seal groove will also but it is still the same basic sketch so it could be an Inventor sketch block.
 
On occasion you may want to link dimensions of a sketch block to other feature sketch dimensions.  Using the parametric table you can write formulas that use the sketch block dimensions to control dimensional values of other feature sketches.  This is shown in the table below.

If you would like to work with the sketch block dimensions graphically you have a problem.  The problem is you cannot see these dimensions unless you are editing the sketch block itself.  This does not help you link them into other sketches using a graphical method.  If you would like to make the sketch block dimensions appear in the sketch in which it is being used in, edit the sketch, then right click on the sketch block folder entry and select "Dimension Visibility" from the context menu.

The sketch block dimensions will show up in the graphic display.

 

If you want to show the dimensions of another feature sketch at the same time, right click on the earlier feature and select "Show Dimensions".




You now have the ability of parametrically sharing dimensions from the sketch block to the other feature sketch simply by selecting dimensions graphically.  In my example I am controling the OD of the flange by the seal groove location and radius.


Try out Inventor sketch blocks and discover ways your design could benefit.

How to Add Synchronous Belts to Inventor Design Accelerator

Designing synchronous belt drives using the Design Accelerator in Inventor makes the task a very simple process.  Not only does the application design and model the drive components but it will do the required calculations to make sure your drive will transmit the required horsepower or torque.  The only regret I hear from designers is that the database does not contain all the desired synchronous belts or there are large gaps between the database size listings.  This article will show you how to add missing belts to the standard database.

The first step is to locate your Inventor default design data folder.  If you are using the default one installed with the software, you can quickly determine the folder location by selecting Application Options, then the Files tab.  Look for the Design Data folder location. 

If you are specifing a special company design data folder location using your Inventor project file, make sure you look at the project file settings to locate it.  It will be under Folder Options.

 
Browse to the folder containing the synchronous belt tables.  You will be looking for the .XML file named for the series of belts you are editing.  In my case, I am adding "H" section belts.  If you are unsure if you have the right file, there is a .JPG file of the same name you can preview to verify the you have the correct belt series.  At this point, you may want to make a copy of the .XML file you are going to modify just in case.
Using your favorite XML or text editor, open the file.  Scroll down to the area where you wish to add your new belts.  Previewing the entries you will easily see how the entries are configured.  In my example below, I am looking at a 330H075 belt.  It has 330 mm long, has 66 teeth and is an "H" section belt .75" wide.

Next thing you will need is a good source for "H" section synchronous belts to make sure you are adding belts which are readily available to purchase.  A quick Internet search will give you many choices for vendors.  I want to add a new entry for a 340H075 belt so I would place it between the 330H075 entry and the 360H075 entry already in the database.  Copy and paste an existing entry and change the necessary information to match your new belt.

Save the XML file and you are done.  Back in Inventor you will find the new synchronous belt size is now available.  If you do not see it at first, close and open Inventor to reload the database.

V-Belts can be added in the same manner to the V-Belt database.  In the entry below, A38 is the size callout, 39.3 is the length of the belt in inches and 0.87 is the belt length correction factor.

 

IMAGINiT Tech Tip | Autodesk Inventor Boss Command

In this Tech Tip, we are continuing our deep dive into the Plastic Part commands of Autodesk Inventor.  This time around we are going to take charge of our plastic parts with the Boss command.  At the end of this post you should be able to tackle tough plastic part designs...like a Boss.  This tool is just about the best thing for plastic connection methods for Autodesk Inventor designs.  What is fantastic about it as a tool in general is that includes so many options for building a Boss feature that eliminates long history trees in your model browser.  This command will build in one command what Extrusions, Revolves, Drafts, Fillets and Hole would do otherwise.  First, lets turn on the Plastic tools.

The first step in the Boss command is to setup where your reference points will be.  That can be done with Work Points or sketches.  In my example, I have a sketch between the two solid bodies that would be the top and bottom halves of my plastic design.  I place two sketch points and I'm done.  You can have one point or ten, doesn't really matter, each point will represent a boss and can also be deselected in the command if you desire.  When you start the tool you get one of the most advanced and complex command boxes inside Inventor.  Here is a look at just one Tab on one of the two options inside Boss.

From these dialog boxes we can build a Head side and a Thread side. We have options here for Stiffening Ribs, fillets all over the place, drafts, and offsets.  So if this dialog makes your head spin a little bit, don't worry you can also use an intuitive grip system built into this tool.  While in the command, simply go to your preview geometry and start pulling on things.  Whatever you can grab whether it be an edge or a vertex will change your inputs in the dialog at the same time.  Here are just a few examples below.

Granted these will need to be done as two separate Boss commands though.  That is easy enough to accomplish as you probably already know.  After you finish your Head or Thread side, simply share the sketch or make is visible from your model browser and then run the command again.  The inputs you had last time will stick and make your opposite side of your connection that much easier to create.

So lets watch some video of the whole process here and try it out with the sample files below.

 

Download Plastic_part_boss

Download Plastic_part_boss_done