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Tag Archives: Inventor

Reviving Inventor’s Design Checker – Making it work for you

In case you have not seen it yet, the (subscription-only) Inventor Design Checker tool is a potentially massive time saver when it comes to checking on the conformance of modelling data to a known (company) standard.

I will not be covering how to use/set it up here since the instructions can be found (in brief) online or in detail in the accompanying help (.chm format) documentation, but suffice it to say it’s really easy to check a whole plethora of common modelling errors/omissions.

I have previously posted about my desire to use the Inventor Design Checker (IDC) to check pre-existing model datasets using this tool, but, if you have used the tool already, you will notice that it has one (to me at least) fatal flaw with the inability to batch process (existing) large assemblies and sub-assemblies.

Because of this flaw, I had ignored the tool for over a year when a series of events led me back to discussing it with the very knowledgeable Adrian Salariu. I praised his post on Inventor Pipe Clips and he then replied to my Google+ post on the subject of the IDC stating that he had previously used it to check a large assembly structure without using iLogic or the API.

We subsequently discussed this further using Google Hangouts and, after understanding how Adrian had accomplished this seemingly impossible goal, here is my guide on using the Inventor Design Checker for batch processing large assemblies:

Preparation for Batch Processing with Inventor Design Checker

There are a huge number of checks that available to use with this tool, and whilst there are too many to mention in detail, the one issue we encounter more than any other in provided-to-us Inventor datasets is “under-constrained-sketches”.

This error ranges in severity from one or two dimensions/constraints missing within one sketch in a part file to (the worst I have seen) 150 of 180 sketches being under-constrained within one part file.

Obviously in the latter case, the only option left to us was to take the original paper drawing data and re-draw the Inventor part from scratch as attempting to piece together a part with around a 70% broken sketch count was simply a non-starter.

Once you have agreed upon a set of company standard checks that you wish to run, the procedure for running the tool as a batch process is relatively simple.

Ensure that “Enable LiveCheck” is selected:

Inventor Design Checker - Enable Live Check

Then double-check the profile you wish to use:

(In my case remembering to turn on the previously mentioned “Under Constrained Sketches”)

Inventor Design Checker -  Under Constrained Sketches

Also remember to add Default iProperties you wish to have checked:

Inventor Design Checker - Default Properties

Save and exit the Design Checker Profile tool, then close Inventor.

Now we need to think about the origin of any files we wish to check, since there are a number of pointers I have discovered that could shape the way you use this tool:

  • Are the files Vaulted?

OR

  • Are the files part of a pack and go?

OR

  • Are they included on an email/CD/DVD?

If the answer to the above is a. then skip to (Vaulted Files).

If the answer to the above is b. then skip to (Pack & Go Files).

If the answer to the above is c. then read on:

In the case of emailed/DVD-based files, simply place them somewhere within your existing Vault folder structure.

Make sure to unset Read-Only on these files and (to prevent missing file errors) open their parent assembly with Inventor. This ensures that (if Inventor is unable to find them) Inventor will download the latest copy of any Content Centre files referenced by this assembly.

Once again, close Inventor and skip ahead to (Processing files using Task Scheduler).

Vaulted Files

Vaulted files can be treated similarly to number 6) above, but with the caveat that if they are in a lifecycle-released state, the IDC results will not be saved to the files in the Vault.

If non-saving of the files is not an issue, for instance if you simply want to report on pre-existing, Vaulted, locked files, then simply do a “Get” at the parent assembly (remembering to tick the “Children” option) and download the latest files from Vault. Then unset Read-Only and open the parent assembly as per step 7 above.

Pack & Go Files

Pack & Go Files should already be writeable, but it is best to check as the IDC will fail on any missing or read-only files and repeated failures will result in the process stopping completely.

Depending on the settings used when creating the Pack & Go, there may or may not be included the relevant Content Centre files, so it is worth setting the Pack & Go project file as current and opening the top-level assembly to force Inventor to get all missing Content. (Of course, Inventor may not be able to retrieve some items in which case an email to the Pack & Go source is likely required.

Processing files using Task Scheduler

With all the necessary files downloaded and ready to be processed, open the Inventor Task Scheduler from the Start Menu -> All Programs -> Autodesk -> Autodesk Inventor (year) -> Tools -> Task Scheduler.

Create a new “Update Design” task:

Inventor Design Checker - Task

If you can’t select a project file, then simply select a folder to use, or even an assembly file:

Then tick the “Immediately” (Assuming you want the task to run straight away!):

Inventor Design Checker - Task Folder

Next, click “Options” and tick the “Total Rebuild” option. (This may or may not be necessary, it was something Adrian & I discussed and we agreed it was probably best to turn this option on):

Inventor Design Checker - Task Run Immediately

Finally click OK to close the Update Design Options and then, if you are happy with the settings you have selected, click OK on the Update Design dialogue.

Inventor Design Checker - Task Total Rebuild

Awaiting the Task Scheduler results

Once the process is running, you will see different “speedometer” icons appearing on-screen whilst the task completes:

Inventor Design Checker - Task Running

Inventor Design Checker - Task Running 2

These different icons display the different checks that have passed/failed within the IDC dataset.

Once the task has completed you will see something similar to this page:

Inventor Design Checker - Task Running 4

The “Red Cross” denotes that the task completed with some errors. In the case above, the most-recent task only had three errors:

Inventor Design Checker - Task Error

Now it is simply a matter of right clicking the completed task and selecting “Create Report”:

Inventor Design Checker - Task Create Report

Then select the filename/path for the report and click OK:

Inventor Design Checker - Task report filename

The report will open and because we ticked the “Errors Only” option will only display errors from the Task Scheduler process:

Inventor Design Checker - Task Report

With the Scheduled task complete, we can now reopen Inventor and begin to interpret the IDC Results.

Inventor Design Checker Results

Open the top-level assembly checked by IDC and you will see the speedometer as shown below:

Inventor Design Checker

The number displayed within shows the number of files that have failed checks. Ideally, this would be zero, with the dial(s) fully green as per this part:

Inventor Design Checker - Results

The exclamation marks shown in the image above are highlighted within the report as “Accepted Failed Checks” and have accompanying remarks from the user (in this case me) explaining what the Accepted Failed Check means.

Inventor: Top Ten iLogic & API Tips

Here are my Top Ten Inventor iLogic tricks. I have included some mentions of the Inventor API and SDK too, since they go hand-in-hand.

Forums, forums, forums

When working with Inventor iLogic, it is important to remember that for the most part, none of what you are likely to create will be “entirely new” code. There is a good chance that somebody on the Autodesk Forums will have either already used the methods available (within iLogic) to do what you want to do with them, or at the very least be able to offer pointers as to how to achieve your goal.

The Inventor API team are always on hand to aid with a specific question and the Expert Elite will occasionally chime in as well.

A good starting point is the Inventor customization forum:

Inventor Customization Forums

In particular, the search function (circled above) is one of the best ways to get started. Always make sure to include iLogic in the search string.

Inventor SDK

One of the most useful (and often overlooked) repositories available to even a seasoned iLogic user is the Inventor SDK. Normally available here:

C:\Users\Public\Documents\Autodesk\Inventor 20##\SDK

It comprises two installers:

Inventor SDK

User Tools

This installer contains the following tools:

Inventor SDK UserToolsThe titles of which should be self-explanatory. 😉

Developer Tools

This installer contains the following tools:

Inventor API developer tools installed

It is worth noting however that without even an Express version of Visual Studio installed, you will receive the following error and be unable to proceed with the installation:

Inventor API developer tools no Visual Studio errorEvent watcher sample

Assuming you did have Visual Studio installed; one gem in the Developer Tools -> Tools folder is the Event Watcher, a standalone app that is especially useful if you want to see what commands are firing within Inventor when using the Inventor UI.

I have previously used this tool to discover and subsequently intercept the “file close” and “file save” events for example.

Keep It Simple, Stupid.

When working in iLogic, it is very easy to end up with an enormous codebase; and whilst this may seem like “do as I say, not as I do” I have in the past created iLogic routines with 500+ lines of code. It is not something I would recommend to anyone starting out. The easiest way to keep things simple is to limit each method to an absolute maximum of 10 variables. I.e. objects you define yourself:

Inventor API Variable CountThe above is a good example of a limited number of variables leading to easily maintained code.

Another tip is regarding named objects you create; sometimes in a large iLogic rule, you will find an error, which results in a useless dialogue from the Inventor UI. Often, this sort of error can be as simple as a typo caused by an overly complex object name. Turning “Option Explicit on” is one method to eliminate these errors before running the rule.

Debugging

A quick way of debugging iLogic code is to place message boxes throughout the rule:

Inventor iLogic messagebox.showThis gives a nice prompt within the Inventor UI that things are running as planned.

I do not recommend including them within a (potentially long running) loop, unless you like clicking the mouse waiting for said loop to finish that is.

Visual Studio

Visual Studio Express is the minimum required to install the a fore-mentioned Developer Tools and is especially useful if you are serious about working with the Inventor API.

Among its many attributes are:

Intellisense

Autocompletes code and can suggest options as you type.

Break Points

These function in a similar way to the message boxes we discussed earlier, but allow the developer to step through the code line by line.

These are both things that Inventor iLogic is sorely lacking, but which is an unlikely implementation unfortunately.

Option Explicit on

A trick I picked up because of this topic of mine is that although VB.NET and thus Inventor iLogic is happy for you to use the following statement:

You will see (as in the case above) strange results within the Inventor UI.

The correct method to use for the above scenario is thus:

Notice the addition of the Type Name Constant preceding the link Object above. To help detect these constants in code, you simply add “Option Explicit On” at the top of the iLogic Rule. This will Force explicit declaration of all variables in an Inventor iLogic rule.

Commenting

Commenting code is often something that is either forgotten or over-used. For instance, when naming objects, there is no need to comment every variable, provided each uses a sensible name. For example:

Dim selectedfile As String = String.Empty” Would not require a comment whereas:

Dim a As String = String.Empty” Would require a comment to denote what ‘a’ means.

Granted, for a small piece of Inventor iLogic it may not be necessary to comment anything, but let us say for instance that you write a comment-free iLogic rule that works so well you do not need to update it for 6 months.

When you next attempt to edit this piece of code, the lack of comments will likely mean spending half a day or more getting to grips with what the code is doing.

Another trick that Visual Studio has up its sleeve (which would be useful in Inventor iLogic) is the ability to auto-expand any instance of three apostrophe characters preceding a method into a block of text resembling this:

Visual Studio Autocomplete CommentsObviously, if you have installed a copy of Visual Studio, and you want to include this kind of commenting, you can copy the header that defines your method into a vb.net class open in Visual Studio, hit apostrophe three times on the line above and it will expand into the layout seen in the image above.

Built-in tools for user ease

For beginners, typing logic statements within iLogic is sometimes a difficult idea to get to grips with.

The iLogic “Edit rule” window does an okay job of highlighting the most-used of these:

iLogic Edit Rule dialogue keywords dropdownThere is also the Operators drop-down:

iLogic Edit Rule dialogue keywords dropdownClicking any of these dropdown items inserts them into the iLogic rule window.

Snippets are your friend

The Snippets available in the iLogic Rule Editor are (by me anyway) an underused addition to the iLogic toolset:

iLogic Edit Rule dialogue snippetsSnippets allow the user to create iLogic rules with minimal searching of the Inventor API documentation.

The snippets included by default allow for simple things like iProperty changes, feature suppression and mathematics through to more advanced topics like running other iLogic rules or even vanilla VB.NET code.

Custom snippets contain parts of actual rules, which you can place into your rules and use them without any modifications:

iLogic Edit Rule dialogue custom snippetsOne of these snippets even allows you to make Inventor talk to the user.

Vaulted iLogic is Good iLogic

Lastly, I find an easy way of creating a repository of iLogic rules is to simply create a sub-folder in Vault and check the files in.

This way, any time you wish to make a change to the Rule in question, you first have to check the file out, and then check it back in when complete. This builds a revision history similar to that which you might see on www.github.com or other similar service.

Autodesk Manufacturing 2016 Product Launch

Autodesk has officially released (April 13, 2015) their Product Design Suite and Factory Design Suites for 2016, in concert with their Simulation software lineup, and Inventor HSM. This package represents a very large range of solutions for its manufacturing industry customers, and includes some great updates to existing products as well as a few new features too.

Autodesk Inventor took the Lion’s share of improvements in what the company is calling an open, connected, end-to-end seamless product development ecosystem. The following are a few highlights from these portfolios.

Product Design Suite (PDS) and Inventor

Recently, we detailed the enhancements in Autodesk Inventor 2016; 387 additions and valuable enhancements such as multi-body sheet metal and model to free-form tools. One addition that stood out was the 3D Printing Environment within Inventor. This allows users to prepare their components for specific vendor’s machines, orienting and partitioning their parts in print spaces that are too limiting. The partition tools include alignment tabs, and the ability to reposition the remaining portions of the part in the void areas of the printer’s effective printing space. Watching the company’s demo of this functionality was kind of cool.

Autodesk Print Studio 2016

Once a print is prepared, users can then send the oriented parts from the 3D Printing Environment to Autodesk’s new 3D Print Studio, an application that helps users build supports and prints the project directly to the large list of known commercial printers.

AnyCAD, Autodesk’s name for their new technology for importing and maintaining most popular CAD model formats inside Inventor assemblies. This allows users the option of importing almost any CAD model for use in their designs, and maintaining the relationship between the original file and the model. If the original file is modified (or overwritten), the imported model is updated dynamically.

Autodesk Inventor 2016 AnyCAD

Buzz Kross, senior vice president, Design, Lifecycle and Simulation at Autodesk noted:

“The new AnyCAD technology in Inventor alone is worth moving to the 2016 version, but we’re also improving every part of the product workflow from concept through product delivery to help companies meet the challenges that lie ahead”

 

Watch Scott’s great video of AnyCAD in action.

 

Other really nice areas of improvement include Sheet Metal environment, 2D Sketching, Drawing Environment, and Presentation Environment (yes, believe it or not).

 

Product Design Suite Software Titles

PDS Premium includes:

  • Inventor
  • AutoCAD( + Mechanical)
  • AutoCAD Raster Design
  • ReCap
  • Vault Basic
  • 3ds Max Design
  • Navisworks Simulate
  • Showcase (downloaded separately)
  • 3D Print Studio
  • Fusion 360

PDS Ultimate adds:

  • Inventor Professional
  • AutoCAD Electrical
  • Navisworks Manage (replaces Simulate)
  • Alias Design (downloaded separately)

 

Factory Design Suite

Additional enhancements for Factory design Suite include:

  • Batch convert legacy CAD items into Factory Assets
  • Quickly convert AutoCAD facility layouts to 3D in Navisworks.
  • Point Clouds display laser scan location map and synchronize across AutoCAD, Inventor, and Navisworks.
  • Create Factory Design Suite assets from Point Clouds

Factory Design Suite Softare Titles

FDS Standard includes:

  • AutoCAD( + Mechanical +Architecture)
  • AutoCAD Raster Design
  • Factory Design Utility
  • ReCap
  • Vault Basic
  • Showcase (downloaded separately)
  • 3D Print Studio

FDS Premium adds:

  • 3ds Max Design
  • Navisworks Simulate
  • Inventor

FDS Ultimate adds:

  • Navisworks Manage (replaces Simulate)
  • Inventor Professional

The Complimenting Simulation and InventorHSM

I’m tempted to call these the landscape after all the money the company has sunk into the technologies. Think back 5 or so years ago and compare… You can’t; there was nothing there.  Autodesk’s end-to-end manufacturing solution is intertwined with continually expanding simulation and CAD/CAM software solutions.

Simulation Portfolio

The Autodesk Simulation portfolio for 2016 has a few changes you don’t want to miss as well as a brand new application. We have more details here.

Inventor HSM

We still do not have the complete picture for the changes in Inventor HSM, but there is one really sweet addition to the product, and more information coming soon. What we can say is…

Autodesk Inventor HSM 2016 gets Turning!

Autodesk added the much awaited turning capability to InventorHSM. The turning addition includes traditional toolpaths with facing, roughing, profiling, grooving and drilling operations. The applications support programming for twin-turret and twin-spindle lathes, plus mill/turn machining.

Autodesk InventorHSM 2016 Gets Turning

What does this mean for Subscribers?

I think Inventor’s improvements alone represent a significant value to engineers and their customers (I won’t rehash these here), and are worth the costs of renewing. I cannot personally speak for specific enhancements within the remaining titles in these suites, but I can attest to the level of detail applied to Autodesk Inventor, and how happy I was to see this much attention paid to a veteran product that we depend on.  Potentially more wonder and technological goodness surrounding Inventor are on the horizon, but I am under oath of silence and secrecy… (first born child and all that).

The integration of Inventor and Nastran In-CAD speaks to the company’s connected, all-encompassing mantra. With regard to the complete end-to-end digital prototyping (and physical prototyping), Autodesk’s Simulation offerings for 2016 hold a few nice features as well. More on that is coming soon.

 

Autodesk Software Information and Downloads

Autodesk Product Design Suite

Autodesk Factory Design Suite

Autodesk Inventor HSM

These products are available now!

Images courtesy of Autodesk, Inc.

 

Autodesk Inventor 2016: What’s New Review

This year Autodesk showed considerable effort towards caring for their existing user base, by adding 32 user requested enhancements in this release, almost 4X that of 2014. There are changes in almost every area of Inventor; from tiny improvements to dialog boxes to complete workflow overhauls; a new rendering engine was added too. The list was really long this year, and quite impressive actually. All we could do is hit some high points in this summary.

Unfortunately, not all features were extended to Inventor LT. We noted as many as we could determine with (*nLT).

User Interface

Various User Interface (UI) features have been tidied. From countless dialog box tweaks to workflows, changes include:

  • Hide all sketch dimensions
  • Import/Export iLogic external rules configuration (*nLT)
  • Numerous Visualization changes
  • All lighting styles are now associated with (IBL) Image Based Lighting.

New 3D Printing Environment

Position your design within the designated printer space and print the components directly from Inventor.

Inventor 2016 3D Print

  • Direct editing in this environment doesn’t modify the original geometry
  • Oversized components can be partitioned
  • List of commercial 3D printers

Sketch

  • Identify sketch plane source. FINALLY!!
  • Create tangent dimensions between curved geometry
  • Enhanced 3D sketch wrapping and projection

Inventor 2016 - Show Sketch Input

Parts

Parts look really exciting this year.

  • Boundary Patch no longer requires closed edge selection
  • Mirror and Pattern support multiple solid body selection
  • Create nonlinear patterns for solid bodies
  • Copy / Paste is now available from the Parameters dialog context menu
  • Surfaces used as parting lines
  • Ruled Surfaces have been added. FINALLY!!

Inventor 2016 - Pattern MultiSolids Inventor 2016 - Ruled Surface

Sheet Metal

Sheet metal is my favorite item this year; well at least so far. Great improvements include multi-body support, new features, 0-bend radii much more.

Inventor 2016 - Multibody Sheetmetal

Check out the details in our first Inventor 2016 New Sheet Metal Features Test Drive.

Freeform Environment / Edit Form

Freeform command activates a Ribbon tab providing full access to the environment.

  • Cool new Convert to Freeform command
  • Work features accessible from Ribbon tab
  • Numerous new commands and features available
  • Intelligent body management

Inventor 2016 - Convert to Freeform

Assembly

  • Analyze Interference improvements
  • Tube and Pipe(*nLT) – File names for Fittings customizable and part numbers populated in Parts Lists
  • Assembly conflict zoom-to

Color Override in Derived Components

‘Use color override from source component’ option added to Derived Assembly (*nLT), Derived Part, Make Part, and Make Component dialog boxes. A global override is available in Application Options.

Drawings

The Drawing Environment received a huge share of attention this time round. Numerous view related workflows have been cleaned up or moved to create a more direct approach of manipulation, as well as many annotation enhancements that were needed.

  • Add projected geometry to view sketches
  • New Reflection Environment settings in the drawing Document Settings – apply specular effect and specify Reflection map in a drawing (.idw) file.
  • New Hidden Line options for Content Center and Sheet Metal
  • Drawing sketch creation is now similar to creating model sketches
  • Merged Format for Dual Hole notes
  • Initial View Scale added to title blocks
  • Transparent components in Drawing Views
  • Create Drawing View from Any Open Model, then current model view orientation and representation are carried over

Overhauled Base View Creation and Editing

The In-Canvas Base View creation tools simplify workflows associated with base and projected view creation. Initial View Scale is set to a best fit and can be changed by dragging the corner to produce the new scale. Direct editing of orientation is now available, as well as a slew of refined features throughout the interface.

Inventor 2016 - Drawing Improvements

Annotation Enhancements

  • Double-click direct editing of symbols
  • Feature Control Frame enhancements
  • Split Leader corrections
  • Single segment leader option
  • One-step leader alignment
  • Symbols list reorganized and enhanced
  • Surface texture symbols updated
  • New external Sketch Symbols Library

Drawing Balloon Enhancements

Balloon creation has been enhanced, including Balloon alignment tools, split Balloons, selection and more. Custom Balloon styles can be created too.

Inventor 2016 drawing balloon improved

New Text Options

Text editing finally received some enhancements and a revamped dialog box, including bullet lists, text case, Graphics Window preview, and much more.

Inventor 2016 new drawing symbols list

Studio Visualization

  • New IBL Lighting Styles added and all custom styles automatically associated with IBL

RapidRT is now the rendering engine for Inventor Studio

Enhanced render quality with additional features:

  • Time duration/iterations/unlimited mode
  • Lighting and Material Accuracy modes

Inventor 2016 Studio Render Enhancements

Presentations (*nLT)

Presentations have been excluded from enhancement since Inventor Publisher arrived…. This year offers some relief:

  • Trail creation and editing enhanced
  • Component selection simplified
  • Enhanced Representations support
  • Triad Manipulator modernized and can be aligned to component geometry
  • Auto Explode improved and added to Ribbon

Tweak Command Enhancements

Tweak Components command is redesigned to include direct manipulation. A mini-toolbar is available with new commands including Undo option.

Inventor 2016 Presentations - Default Trails

Dynamic previewing of tweaks now occurs, and components are rolled back during tweak editing to preview the changes.

  • Tweaked component selection sets amended dynamically
  • Enhanced Trail editing and manual creation
  • In-Canvas editing of distance and angle

Interoperability

Autodesk continues to merge the seams between CAD model versions, with some focus on AutoCAD and non-native formats.

  • Simplified importing of non-Autodesk CAD files

Associativity

Associative CAD file import maintains and updates links with:

  • SolidWorks
  • CATIA
  • NX
  • Pro-E/Creo
  • Alias

AutoCAD Electrical and Inventor (*nLT)

A New Electromechanical Tab has been added to the Ribbon. The New Electromechanical link between Inventor and AutoCAD Electrical provides smooth data exchange and update between the two.

Other Enhancements

  • Multi-thread support (Single processor only)
  • 64 bit only support for Inventor 2016 through Win 8.1 (LT still supports 32-bit)

Detailed What’s New Posts

Autodesk Inventor 2016 Now Uses Any CAD format

Sketching a Circle Around the Competition with Inventor 2016

Autodesk Inventor 2016 – Drawing Environment Improvements

Presenting Inventor 2016 (What’s New With Presentations?)

Autodesk Inventor 2016: Sheet Metal New Features

Thank You!

Thank you to our team for pumping out this series of posts:

There will be plenty more to come about Inventor 2016 in the coming weeks and months.

Autodesk Inventor 2016 Now Uses Any CAD format

Ok, not quite any CAD format, but all the really important ones are covered; Solidworks, CATIA, NX, Pro Engineer and PTC Creo. Hey, what did you say? you may be asking… Yes Autodesk Inventor 2016 will now natively import and maintain associativity with all major CAD file formats. BOOM! Now that guys & gals, is a game changer for the wider CAD / CAM industry.

Autodesk Inventor 2016 Multi-CAD

Why’s it a Game Changer?

There are plenty multi-CAD workplaces knocking about, whether that’s because of mergers, legacy decisions in different departments or a heavy reliance on contract design staff. But this is also a big deal for the CAM users out there, those guys are receiving various data formats from all their clients every day… and they are also subject to in process change just like everyone else is.

In the way the Navisworks changed the way multi-disciplinary design review was carried out forever (and it’s competitors), Autodesk Inventor’s Multi-CAD functionality promises to do the same for the modelling process itself. Yes, PTC got in there first with Creo 3.0 delivering their Unite Technology supporting Solidworks, CATIA and NX files. Inventor 2016 supports those same file formats, as well as PTC Creo, Pro Engineer Wildfire and Autodesk Alias. I never got the opportunity to try out Unite in Creo 3.0, so I can’t compare real-world functionality unfortunately.

How does it work?

I have absolutely no clue, beyond knowing the translators in use are from a 3rd party* (which other CAD vendors will also be using) and a heavy dose of wizardry from the Autodesk developers! What I do know, is you can open any of the supported file types, either parts or assemblies, straight into an Inventor part or assembly. You even get to read the BOM of the source files via Inventor’s Bill Of Materials dialog. Check out this video to see how it’s done:

Does it work?

I’ve only been able to test it using datasets created in Solidworks 2015 SP1.1. So I can’t speak for the other file formats at this stage, but the harsh reality is there are issues. Bearing in mind that there is a lot of Black Magic going on here, it is hardly surprising. However, this is the first release of the technology and I have no doubt that PTC’s Unite Technology will have issues as well. But the great thing is, both of these companies are having a go at breaking down the barriers put up by competing CAD file formats.

The problems I have encountered initially are:

  • 80% of the time a projected edge from a Multi-CAD source will fail on update when the source model geometry around it changes.
  • Geometry changes within the boundary of the Multi-CAD model work better than changes which result in the overall model size changing.
  • Assembly Joints & Constraints are a bit hit & miss at release, but those relationships are more stable than sketch projections are.

So basically, if you stick to a bottom > up modelling workflow with these components you are more likely to succeed than using a top > down approach.

I did manage to program a native Solidworks part file, inside Inventor HSM though and maintain an associative relationship:

DWG Underlay

Another excellent feature which arrives under the ‘Multi-CAD’ banner, is the AutoCAD DWG Underlay. I was honestly speechless when I saw this for the first time. Having worked with Inventor in the Super Yacht interiors industry for 10 years, I’m acutely aware of how poorly Inventor handles large amounts of AutoCAD 2D objects. General Arrangement plans are highly detailed beasts in the marine (and aerospace) industry, because they’ve historically been used to sell yachts there is a lot of stylized line work. It can be a pain to clean it all up, only to receive another version the following week. God I wish I had this tool in the past. Feast your eyes on this:

* Digging through the Autodesk Inventor Trademarks and credits declaration, you will find a reference to CADCAM-E.COM. Credit to a very curious colleague of mine for finding that!

Autodesk Inventor 2016: Sheet Metal New Features

My favorite addition to Inventor 2016 is most likely Sheet Metal. That’s not to say that other great enhancements were less impressive, but that sheet metal design has been waiting on these improvements for some time.

Autodesk Inventor Sheet Metal Multi-Body

These improvements include:

  • Zero bend radius support
  • Material thickness detection in standard part to sheet metal part conversion
  • Punch tool shows center selection count
  • Dialog Enhancements

Multi-body Support for Sheet Metal

This is the cat’s meow; Top down workflows through Make Components and Make Parts allows users to write out components and generate separate flat patterns.

New Solid body option includes Face, Contour Flange, Contour Roll, Lofted Flange, and Split, with multi-body workflows for many others.

During the ‘Convert Part to Sheet Metal’ command, sheet thicknesses are automatically determined by detection from a selected face when prompted.

A Quick Run-Through

I needed to put something to the test and then show here, because most of my readers are “all text and no pictures makes Jack bored silly”. I didn’t have but an hour to spend, so I threw this seal mount together, and later decided to integrate it into a bulkhead instead.

Sheet Metal Part Creation

I started with a 2D sketch, from which I turned a contour roll of 0.063” aluminum with 1.5” flanges in a single motion. I unfolded the half circle shape, so that I essentially had an L-angle, and added two mating end flanges, as well as the bolt and rivet holes by rectangular pattern.

Finally I refolded the structure (still amazing and cool that all the features hold together), and added a circular pattern of two components to copy the structure around the circle, making sure to pick the New Body option.

Autodesk Inventor 2016: Sheet metal make components

Inventor created a mating duplicate body, both of which I quickly wrote out to an assembly using the Create Components command. As you might imagine, the two components were placed and grounded just as if they were regular part bodies.

Flat Patterns

I remembered reading how flat patterns were associated with each individual part file, so I edited one, and sure enough, the option to Edit Flat Pattern was there.

AWESOME!!!!

Autodesk Inventor 2016: Sheet Metal Flat pattern

Another Body

I returned to the multi-body sheet metal part, and turned off the lower seal ring support. I created a Face for a new body, and added another contour roll, flanges, and fasteners with typical operations.

Once again I wrote the part out, and used Component Replace to swap the bulkhead into the lower seal ring’s place.

Yep, you guessed it, it worked perfectly.

0 Bend Radius Support

I thought that it would be a good idea to test the 0 bend radius on this odd back and forth operation I had going. I edited the upper seal contour roll, and changed the radius to 0. Everything updated properly. Inside radius was 0, and outside of sheet radius was the sheet thickness.

Autodesk Inventor 2016: Sheet Metal 0 bend radius

Conclusion

I am quite happy to get multi-body sheet metal into Inventor finally, a functional part of the overall design process. Is there anything remaining that needs to be handled?

Sure, like more aviation type manipulations for example. However, these additions are a real winning addition and are something that we can build new workflows from immediately.

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