Opening Mechanical Desktop Files in Inventor 2018

The need to convert Autodesk Mechanical Desktop (MDT) models to Inventor has become less of a requirement since the last version of MDT was released in 2009 but there is still the occasional need that pops up from time to time.  Autodesk has written a version of MDT 2009 for use with Inventor 2018 to make the task easy and I would like to use this article to outline the process of getting set up to do so.  One of the great features of this MDT 2009 to Inventor 2o18 version is that not only will it convert part models it will also handle MDT assembly models converting all the parts as well as sub-assemblies in one operation.  So lets get started.

The first thing you need is a computer running Windows 7 SP1 x64 operating system.  Windows 7 SP1 is required since the MDT application will not run on Windows 10.  You may try and use the Windows 7 compatibility settings in Windows 10 and get it to install and running but Autodesk does not recommend it.  If you are already running Windows 7 SP1 x64, then you are set.  If you are running Windows 10 Professional, you can use the built in Hyper-V utility to create a virtual machine and install Windows 7 SP1 x64 on it.  Hyper-V is also found in Windows 10 Enterprise and Windows 10 Educational.  I found the process of creating a Hyper-V virtual machine easy and straight forward except for the process of creating a shared folder between the host and the virtual machine.  After a little research on the internet, I overcame this hurdle also.

Once your virtual machine has been created and you have installed a copy of Windows 7 SP1 X64, you are ready to download and install both Autodesk Inventor 2018 and the "MDT 2009 to Inventor 2018" application.  You can find the process for installation of both and the MDT 2009 to Inventor 2018 application on this website.  I encourage you to read the complete process before you install either Inventor 2018 or the MDT 2009 to Inventor 2018 application.

If you have your Autodesk Mechanical Desktop 2009 original serial number, you should use that during installation.  If you do not have it, use all zeros as the serial number, this will secure you a 30 day trail of MDT 2009.  If this is not enough time, you can contact Autodesk to secure more time.

There are no special Inventor project file requirements to do conversions, you can create one from your existing company Design Data and Templates or use the default Inventor project file.  The conversion process will allow you to configure the templates and folder location for the conversions as well as other settings.  I will walk through a conversion later in this article.  Before attempting to open any MDT file in Inventor 2018 and use the conversion process, you MUST run MDT 2009 at least one time after installation.

I will now step through the conversion process.  Open up Inventor 2018 and make sure your have your project file selected.  I am using my companies Design Data and Templates so I can make sure the conversions are ready for my company's Vault and other applications.  As you can see I have a very simple folder structure on my virtual machine setup.  One folder for the MDT files to be translated and one folder for the finished translations.

Next I will select a file from the MDT Files folder that I desire to convert.  The next step is to select the "Options.." icon on the bottom of the Open dialog box and make sure the "Import" option is selected.  If you do not want to do this every time, I suggest you set it as a default by stopping the open process and select "Tools" then the "Application Options" from the Options panel.  Select the Drawing tab and select "Import" as the default for opening Non-Inventor DWG files.

The first dialog that Inventor presents is the beginning of the configuration sequence.  One thing right off the bat is to remember to save your configuration setup so you can simply select it the next time you start the translation process.  This is done at the end of the configuration settings and selected the next time at the beginning of the process.

Inventor will already recognize that you are opening a Mechanical Desktop File so select "Next" to continue.  In the Mechanical Desktop Model/Layout Import Options dialog box you can select what you want to import.  You will probably select "Parts and Assemblies" in order to import the MDT model into an Inventor model but you can also select to have one or all the available MDT layout views imported and translated to Inventor 2D drawing files.  By the way, the "Model" and "Layout" tabs can be selected as well as either view can be zoomed and panned for inspection using your mouse.  Select "Next" to continue.

The next screen is full of selections so take your time and study them.  The "Drawings with View Options" and "Mechanical Symbols"  will be grayed out unless you selected to import Layouts from the previous screen.  The settings are up to your needs but a couple I would definitely take a look at.  Under "Import Files Units" make sure the correct units have been detected from the MDT file, if not select "Specify Units" and pick the correct units from the list.  If you want to use your company templates and you have configured the selected Inventor project file to use your Design Data and Templates, you can browse and select these under the "Templates" section.  Make sure you configure them all so your saved configuration will cover all future translations.  One of the most important setting is "Destination Folder" which will be where Inventor will "automatically" save the final translation(s) including all parts and sub-assemblies if the MDT file is an assembly.   Near the bottom right corner you will see the "Save Configuration" icon.   Select this and name and save your configuration to a folder of your choice.  Select "Finish" to begin the MDT translation.

During the translation process MDT 2009 will open briefly, you may notice it in the Windows taskbar.

The translation process will create models with semi-editable features.  I say semi-editable since some feature sketches may be a little weird because of their dimension placement and feature parameters use of lot of the "Isolate" function but you can easily type over these if needed.

One last note before I end.  Autodesk on their website pages describing this application warn that this will be the "final" MDT 2009 to Inventor application so if you need it in the future you will need to use Inventor 2018 and this MDT 2009 application and migrate forward.

Using Inventor iMates with Fasteners

The use of  iMates is far from one of the most used features of Autodesk Inventor for a number of reasons.  The leading one is the time it takes to create iMates or composite iMates.  If your component is used only once or a few times, it hardly justifies the time it takes to create an iMate constraint.  

There is a great use for iMates that is often overlooked, and that is the constraining of Content Center fasteners into your assembly.  Content Center fasteners, supplied with Inventor, are all configured with predefined iMates.  When you select a fastener in an assembly the iMate icons pop up, with a lot of users scratching their heads as to their use.

The symbols you see represent the iMates assigned to this fastener.  I wish I could zoom up on them for clarity but as you will find out, you cannot.  The ones on this socket head cap screw are a mate constrain to the shoulder of the head, a mate to the centerline of the screw and an insert one one of the edges of the shoulder.  Compare the small icons to the symbols shown in the Place Constraint dialog box and you will soon easily recognize them.  They also generally appear near the feature that are attached to.

The process of using them is very easy.  First of all decide which constraint you would use to place the screw in the plate hole.  Most all users will elect to use the insert constraint since it combines two mate constraints at the same time, one between the centerline of the screw and the hole and one between the bottom of the screw head and the surface of the plate where the hole begins.

Once you decide, hold down the Alt key and left click select and start dragging the insert iMate on the screw.  It will turn green as you drag.  At this point you should let go of the Alt key but do not left go of the left mouse button.  Notice the edge of the screw that highlights and also the insertion arrow at the end of the screw.

Continue with you left click drag until you hover over the edge of the plate hole you want to use as the other side of the insert command, it will also highlight.  At this point release the left mouse button to apply the insert constraint. 

With a little practice you can become very fast with this process easily placing screws, washers and nuts in your assembly must faster than using the Place Constraint command.

The one downside in the use of iMates is that you cannot edit the offset value of any iMates, the offset value when they are created is set.  Take the insert iMate I created above.  If I find it in the browser, notice the icon is a bit different than a normal insert constraint, and edit it, the offset spacing is grayed out.

You can use this method of applying assembly constraints on components that do not have previously created iMates but it will take a little more practice, especially if you want to switch the type of assembly constraint being applied on the fly.  I will not go into how to perform this task in this article but you can easily find the process in the Inventor help file.

To finish off, I wanted to post a video of the use of iMates to finish placing the screws, washers and nuts and also placement of the yellow pin, which does not have any predefined iMates.  Remember as you watch this video I am doing the same process outlined above with the Alt key and the left mouse drag.

Solving Inventor Template Style Conflicts

I have been seen many Inventor users encounter the following error every time they create a new Inventor file and simply live with it by selecting OK and moving on.

It normally is more a nuisance instead of a problem but why accept it when the solution is relativily simple.  The first thing to understand how Inventor templates and Design Data are related.  By the way, Design Data is often called the Styles Library so do not confuse them, they are identical.  Inventor templates contain certain configurations for example text styles, dimensional styles, layer settings, etc.  There are a vast number of configuration settings, especially in the 2D drawing template but I will just use text styles for this article.  Inventor Design Data also contains configuration settings for all Inventor template types.  Both of these and their location are declared in the Application Options or in the current Inventor Project file.  I am a fan of using the Inventor Project file to declare the current template and Design Data files and their location.  I have two reasons for this, one I do not want to modify the default Inventor templates or Design Data because I want to always have a clean source if I want to build a new configuration.  Sure I could backup the originals before modifying them but you know how that goes.  The second and main reason is that I can declare a different set of templates and Design Data for different project files.  This does not mean I use a different project files for each company project, I only use one project file for all company work.  Many companies often have to design work for other companies using their templates and Design Data.  If this is the case I can have a project file for each company and each project file declares the templates and Design Data for their work.

Getting back to the reason for the "Style Conflict" error.  If the Inventor template configuration does not match the Design Data configuration, you will get this error.  I will not go into the reasons it happens, I just want to tell you how to solve it.  First of all one person in the company should be in charge of Inventor templates and Design Data.  This person should create a special Inventor project file dedicated to template and Design Data creation.  This project file declares three main things, that the Style Library (Design Data) is Read-Write and the location of the Design Data and and the matching templates.  Note the screen shot of my Inventor 2018 Template Work.ipj file and the marked areas.  If you use the Vault, this project file should be a Single User type.  The red arrow is simply trying to explain that the ".\" entry for Templates location is the same as the location of the project file itself.  Make this project file active.

The next step is to open up the offending template and select the "Update" icon under the Manage tab, Styles and Standards panel. 

You will see the style that is conflicting.  In my example it is only one but there may be many more.  At this point STOP and ask yourself, "Is the Design Data configuration correct or is the template?"  If it is the template, select "Cancel" and read on later in this article.  If the template needs to be updated to match the Design Data (Styles Library) then select "Yes to All" icon near the bottom of the dialog box and then select "OK" to finish.

Inventor will give you the following message which basically says you are updating the template to match the Design Data, the cause of the error.  Select "OK" to continue.

Next, save the template and close it.  Since this is the only template I am editing I will return to the standard company Inventor project file and test my work.  If you have more than one problem template, repeat the steps for each template before switching project files.  

When you open the template file, the error message will not appear.  Congratulations, you have fix your company template file(s).

So now we want to think about what to do if you earlier decided that the template file is correct and the Design Data should be updated to match.  Instead of selecting the "Update" command, you will select the "Save" command right above it.  This will save the template configuration to the Design Data folder.

 

 

Do not forget to choose "Yes to All" before selecting "OK" to be sure you are actually writing the changes to the Design Data.  Since you have written new data to the Design Data folder, all other templates may be out of date and do not match the new Design Data. The original error will appear for them as well when they are opened.  After writing new configurations to the Design Data folder, you must open each Inventor template and follow the "Update" procedure for each outline above.  Remember all of this must be done while using the Inventor project file you earlier created for editing your templates and Design Data.

 

This may sound like a lot of work but it actually only takes a couple of minutes.  The configuration of the original templates and Design Data to match your company standards is the real work and may take you many hours.  By the way when you upgrade your Inventor version all templates and Design Data must be migrated.  The process is similar once you have migrated the Design Data using the installed Inventor Styles Manager.  That could be a new article I will try and tackle later.

 



Part Modeling Mirror Command Improvement in Inventor 2018

This will be a quick article to call your attention to a very nice addition to the "Mirror" command in the part modeling environment of Inventor 2018.  Most all experienced Inventor modelers always design their parts around the origin point so they can take advantage of the default origin places for various operations.  This especially is true when using the "Mirror" command.

The process went something like this, select the feature(s) you wanted to mirror and then the "Mirror" command.  Of course you can reverse the process of selection, it is all a matter of your operational taste.  Then you expanded the Origin folder in the browser and selected the origin plane you are mirroring the feature(s) about.  

Well the origin planes selection icons have been added to the command dialog making it a much smoother process.  The "Mirror" command dialog box is both Inventor 2018 and Inventor 2017 are shown below.

Recalling Vault History using Labels

There is a tool found in all versions of Autodesk Vault that will make your job of recalling Inventor designs a walk in the park.  The tool is called "Labels", but before I jump in and talk about the process of using labels, I want to give you a couple of scenarios just to give you a reason to use this marvelous tool.

Scenario 1: Your company designs equipment in Autodesk Inventor that will go through numerous changes during its usable life.  Let's say the original equipment design was created in February, 2017, the design was locked down and 50 assemblies of this design were shipped soon after.  Now we will turn the clock ahead to July, 2017 and your company determines that the original equipment design needs to be revised and improved for a new customer who has ordered 60 assemblies.  Your company design team is worried about revising the original design files because they may not be able to remember the design as it was shipped for the original 50 assemblies.  What if the original equipment needs replacement parts?  What if the customer who ordered the first 50 assemblies whats some design changes?  This is a great use of the "Labels" command inside the Autodesk Vault application.

Scenario 2: Your company creates a particular consumer product.  The product is originally designed and manufactured in large quantities.  The production design is assigned a model number to identify the particular design.  Well into the production, it is discovered that a small change would increase sales so the engineering team needs to start with the revision of the original design and wonders the best method of retaining the the original model number design while moving quickly ahead on the creation of the newer model required by sales.  They know they must retain the original model's design in order to support their replacement part division as well as making sure they can document the original model for regulator bodies.

Both of these scenarios have a number of solutions but most of them are very time consuming and subject to error, take a vast amount of time and probably will create confusion as time passes and memories fade.  Many companies will simply copy all the Inventor models and drawings to a safe protected folder so they can retrieve them if and when they are needed.  Some companies will create reams of production drawings with the hope they can find the correct one if an older model has to be reconstructed.  The Autodesk Vault offers an effective, quick, and simple solution to these types of situations and the process will not depend on someone retaining past design knowledge for years or even decades.  Vault "Labels" are the answer so let me give you an example to show you how it works.

I will first give you two views of the completed design of my companies product.  The design is finished and all supporting models and drawings have been created using Autodesk Inventor and checked into the Autodesk Vault.  Production will start next week.

The production run is complete and the first 100 assemblies have been shipped.  During the production run, another customer has ordered 250 assemblies of the same design except they want two changes to two different parts, the vertical post and the base.  The engineering department needs the new final design quickly but must preserve the initial design for replacement parts and support of current production. The first step is to create a "Label" in the Vault which essentially is a "historical design bookmark" between the original design and the modifications required for the new design.

A Vault user with "Document Editor (Level 1)", or higher, security logs into the Vault, and selects the "Labels" tool from the Tools menu.

In the Labels dialog box, left click on the "New" icon to open the New Label dialog box.  The first thing it to select the target location of the label.  Using the three dots at the end of the field, browse to the folder containing the completed original design.  This step should point out to your Vault manager the importance of good Vault folder structure and keeping all related design documentation under one folder.   Next give the label a very descriptive name so you can identify it easily in the future along with a description if it will help you identify the label when memories fade or the individual who created it is not available.  Select "OK" at the bottom of the dialog to finish and return to the Labels dialog box.  By the way, the only thing you can edit, once you create a label, is the name and description so take you time and select the correct folder.

Take a second to understand the file count in my label.  The label says that 43 files have been labeled and will be bookmarked at this point in their Vault history.  Why 43 when there are only 21 objects listed in my folder.  Well we must not forget about the visualization files which makes 42 and one Word document attached to the top level assembly calling out the boxing materials needed for shipment.

This is the contents of the Word document so you can see the affect of labels on attachments as well.

The label has been created, a label bookmark of the current state of  43 files has been place in the Vault.  Select "Close" to finish.  The design modifications, required for the new customer, can take place using the original files with the confidence you can return to the current design at any time.  The changes to the assembly, parts and drawings are indicated below and checked into the Vault.  The addition of the indicated line to the Word document have also been checked into the Vault.  The new design is finished and production begins on the second customers 250 assemblies.

We will imagine that some time has passed and then the customer who purchased the 100 original design assemblies calls and ask for 4 replacement assembly bases.  It is time to use our Vault "Label" created earlier.  A Vault user with "Document Editor (Level 1)" or higher security clearance logs into the Vault and select "Labels" from the Tools menu.  The Labels dialog box offers two methods of securing the complete history of the original design.  The "Restore" option will version up all 43 original documents becoming the current Vault version.  This option may not be what you desire since you would like to leave the Vault showing the modified assembly created for the second customer.  You could preserve the current Vault folder version by making another Label, then restore the previous Label.  After completing the changes to the assembly required by customer 1, restore the current assembly label.  This is a decision for your engineering department. 

 Many Vault users will elect to use the second option to do a "Pack and Go" to a separate folder under the Vault workspace and edit from these models and drawings.   Whichever method you choose, an accurate recalling of the Vault history makes the job an easy, fast and accurate task.

I decided to create a current customer 2 design label and then use the "Restore" option.  Once I am finished, I would probably make another label to bookmark the revised assembly for customer 1 then "Restore" the current design for customer 2 using my label.  Once this label was restored, it can be deleted.  This may seem a little confusing but with proper description and names, labels can be managed easily especially if only one in the engineering group handles all labels.

I will only bore you with one screenshot confirming that the label worked but you can trust me, it placed all objects to a new version using the "Label" older versions.

Two things I want to emphasis.  First, Vault labels will not recover a deleted object.  If you have deleted a model and drawing since the label was created, executing the label "Restore" will not bring it back.  Second, you can have as many Vault Labels as you desire, just take my advice and annotate them well.  If you do create and maintain numerous labels and later on your Vault administrator decides to do a purge versions history from the Vault, remember that all versions relating to saved labels cannot be purged.

I encourage you to test Vault Labels on one of your small Inventor assemblies and see first hand how valuable this tool can be.

Editing Design Views the Easy Way

The use of Design Views in Inventor assemblies makes it easy to edit and work with parts and assemblies by turning off, and on, parts and components.  They can control other features of the assembly such as work features, part color, section views and many others.  The normal method of creating design views is to select parts and components in the Browser and either hide them or make them visible.  The attached video will show you a different way to do this using a mini-toolbar specifically designed for this purpose.

You can access the video by clicking here.  I will again remind you that this method only applies to parts and components in the assembly.  I also mention a different method of controlling the saved camera in your design views during the video.

Autodesk Vault File Thumbnails Not Created

I have been in the process of creating a new Autodesk Vault and I ran across a issue I want to tell everyone about and how to avoid it.  I did it to myself because I had not finished my new Vault before I started testing.

The issue was that when I checked in some Inventor test files to test out my new Categories thumbnails were not being created.

With the help of Irvin Hayes Jr. of Autodesk, who responded to my Vault Forum post on the issue, I found my mistake and I would like to share it with you.  As I build a Vault I always start with creating all of my Categories.  After I set up a few and add my Category Rules, I tested.  I, at this point, had never gotten around to assigning an Vault Properties to my Categories and that was my mistake.  Irvin reminded my that I must have at least one Vault Property assigned to each Category to tell Vault to generated property values for the files during check in.  Thumbnails are one of the Vault Properties so since I had not told the Vault to generate file properties, no Thumbnails were generated either.  So after adding just one standard Vault Property to the Category, my problem is solved.

Thanks Irvin!