IMAGINiT Manufacturing Solutions Blog

Replacing Family Template in an Inventor Custom Content Library

Companies build their Inventor custom content libraries for various reasons.  Some will create them to hold their internal custom parts, others will copy existing libraries and change their default part numbers and filenames to suit their company standards.  I would like to give you another reason and that is the ability to add parametric features to your custom libraries.  I am going to show you the simple method of adding parametric features to every member of your custom library family with one easy command.

I am going to create a custom content library of ANSI equal leg angles that contains two parametric features per family member.  The first feature are two slots, one at each end of the angle, that are parametrically centered along the length of one leg. The slots can be parametrically adjusted in size and location during placement in an assembly.  The second feature is the parametric embossing of a part number on the opposite leg of the angle.  Here is a screen shot of my part.

Before I continue, I am assuming everyone knows how I created my custom content library by coping the Inventor ANSI equal leg angle standard library to make it editable.  Drop me a line if you need a separate article on that process.
Next I created an assembly using inch units.  I place a piece of angle, in my assembly, from my new custom library.  I used a piece of 2 x 2 x 1/4 but it is not really important what size you choose.  I hate to work on small parts if I do not have to.  The angle has to be saved as a custom library part so I gave it a name of Angle Template Part just to make it easy to find.  If you would like to use this process on a custom library that does not, by default, save the placed component as a custom part, just select "As Custom" during the placement process.

Open up the part and add your desired parametric features.  Be sure to use the User Parameters already in the model to help you achieve what you want.  I used the G_H (Leg Depth) variable to keep my slot centered for all angles in the family.  Features and parameters are up to you.  You could place bolting holes, cutouts, patterns or addition features anything you desire.

For the parametric label, I used a Text user parameter with values in a Multi-List, assigned it to sketched text, constrained to a certain place on the angle leg, and then embossed it.  When a piece of steel is place in an assembly from my custom library, a quick parameter change and I have a new label.  Save the part, you will use it in the next step.

All of this preparation has lead me up to what this article is all about.  I want to add all of these features and any other modifications such as color, custom properties, etc. to all the members of my custom content library in one quick step.  I saved the part I have been adding to and closed it.  I go into the Content Center Editor and locate my custom library, right click on the family I am editing and chose "Replace Family Template" from the context menu.

The program may give you a warning about replacing the template on a linked library, click Yes and continue.  It will then ask you to select the part you saved out of the custom library and have been modifying, in my case it was Angle Template Part.  After selecting Open, you will see a message "Publish was Successful" and you are done.

The next time you place a part from this custom content family in your assembly, it will have all the features you included in your template part.  Best of all the features are applied to every member (size) in the custom library with only one simple command.  Save your template part so you can add or modify features as needed and follow the same process to update your library members.

This process adds a whole new dimension to Inventor Custom Content Libraries.  See what you can dream up in your design process to take advantage of this process.

 

 

 

Reverse your Presentations in Inventor

When you create a presentation in Inventor, you will be starting with an assembly.  You will be tweaking (moving) components and parts to create what sometimes is called an Exploded View model.  Below is a simple exploded view model.

If all you need is a presentation file to created an assembly drawing view for the purpose of Bill of Material ballooning, then you are done.  If you wish to create an AVI or WMV file for either training or your customer use, you will need to animate and record the presentation.

This brings me to the topic of this article.  You created your presentation by dragging, or specifying a distance, each component or part to create the exploded view.  You can of course record the re-assembling of the model but what if you desire to record the reverse, the explosion of the model.  You want the recording to show the actual tweaking you did to create the presentation file in the first place.

There is a well hidden switch that will do just this.  This switch is located under the "Sequence View" in the Browser. 

Once in the sequence view, right click on the top level Explosion and chose "View as Assembly" to remove the check.  This will reverse the sequence steps in the browser  so the first sequence is actually the first tweak you created.  This switch is a toggle so you can go back to the default method of assembling the components and parts when an animation is run.

The presentation model will not change when you remove the check mark, it will instantaneously re-assembly all components and parts when you start the animation and proceed to explode in the sequence you original created the presentation.  Below is a short video to show this process.

 

Inventor 2016 - Automatic Drawing Plot Scale

Inventor users for years have devised various ways of adding the drawing plot scale to the their title blocks.  They have used mapped custom drawing properties, iLogic routines and prompted entries.  We have wondered why Autodesk never made it a drawing property.  Well the wait is over, Inventor 2016 detects the drawing scale of the first placed view and assigns it to Sheet Properties of the drawing as the property Initial View Scale.

Place this property in your title block and it will pick up the scale factor of the first placed view.  Two things to keep in mind.  One, the scale factor format is identical to the scale factor format you select or type in.

  Two, the scale factor is only linked to the base view (the first placed view).  Changes to projected views are not reflected in the property.  Changes to the base view scale will automatically update the property and removing the view will delete the property value.

I am sure there are some pretty sophisticated iLogic routines out there that will continue to be used but at least now, Autodesk has given all their users a way to capture the scale of the drawing.

Tools for 3D Printing in Inventor

3D printing, as a part of the manufacturing design workflow has made that transition from an expensive process option to a cost effective way to prototype a design. In fact with costs down so much companies are buying their own 3D printers and using them to create and iterate ideas early on, not only to validate prototypes. This is an exciting trend since it allows more creativity during the design process and as a designer myself I always find it rewarding to see the physical result of a virtual model come about. So, with the proliferation of 3D printing in the design workflow and updates to the tools available in Inventor it is a good time to take a look at how to use Inventor to prep a model for 3D printing.

There are a number of useful tools in Inventor for 3D printing such as inspection tools and some handy add-ins but this year saw the inclusion of the new 3D Print environment. No longer do I simply export an STL file and hope for the best. Instead an Inventor model can be viewed in the context of a 3D printer’s print envelope with the ability to make changes so the model will fit.

When entering the 3D Print environment the active Inventor model will display bounded by the print area of the default 3D printer. We can see below that my part is within the envelope of the Autodesk Ember 3D printer in its current orientation. What you are looking at below is a print I made of a toy that is assembled to create a spinning top called a Beyblade.

Usually the tabs in Inventor’s ribbon are laid out so that you work from the left to the right. However, in the 3D Print environment I first need to set the printer that I plan on using to create the print with. This is done in the Print panel using the drop-down arrow under the default Autodesk Ember printer. In the drop-down I can make a selection from the predefined list of common printers or from the Other Printers dialog box.

Once the printer is selected the boundary shows the placement of my part on the printer’s bed. This serves as a check before actually exporting the STL to make sure it will fit. Keep in mind that the printer bed and printer information are not actually output from the 3D Print environment, just the model.

To reposition the model in the printing envelope of the printer I use the Set Orientation and Set Position tools. First I use Set Orientation to rotate the model into the best orientation on the print bed. Selecting either Bed or Wall from the mini-toolbar and aligning a planar face (or work plane) to the bed or selected boundary face on the printing envelope.

Once the model is oriented I can use Set Position to offset the model’s body from a selected face on the printer’s envelope. First I select a printer face and then enter an offset value for the distance to the body. This is repeated with the printer’s adjacent face if necessary.

These tools are nice for visualizing a print before committing to production but so far these features, while helpful, do not provide anything we can’t really do without. However, there are tools in the Modify panel that can help change the model to fit the printable since it is too big.

As you can see above my model is actually extending outside the printable area of the Autodesk Ember print envelope after I reoriented it. Keeping this printing orientation means that I would not be able to print the model in its current state. To change the model itself so it is printable in this orientation I can use the Direct tool to push/pull surfaces as needed to get the model to fit. This tool works the same way as the Direct edit tool does in the Inventor part modelling environment.

Since the Direct tool will actually make changes to my model geometry this may not be the best avenue to create a printable file. The second tool available is the Partition tool which can split the model into two smaller bodies based on a face or selected plane. Then each body can be printed and/or positioned separately.

Unfortunately multiple split bodies will create separate pieces that need to be assembled. The good news though is that the Partition tool can add alignment pins and holes that are used to reassemble the parts once printed!

After selecting the plane to split the part I select as many points as needed on the split plane to automatically create pins. The pins will be created at the selected points based on the depth, diameter and taper values entered in the mini-toolbar. The alignment holes that correspond to the pins will be created automatically on the second printed body from the split plane. Their size is set by the Scale Factor entered on the next line down in the mini-toolbar. This should never be less than 1.

So now I have two bodies from my part file with alignment pins. I can go back and use the Set Orientation and Set Position tools to move the separate bodies individually so that they fit on the bed of the printer.

A major thing to note about the 3D Print modification tools is that they only apply in the 3D Print environment. Once outside of the 3D Print environment the part or assembly model will not have any of the splits and moves made here.

Now with my model ready to print I am almost ready to go. I can select Print Options to set the STL output settings such as resolution and units then visually verify the STL mesh that is created using the Mesh tool. If everything looks good hitting the STL button will export the file for printing using the geometry in the orientation displayed.

Here is a picture of the finished print of the model I used above, printed in stainless steel!

If you have an Autodesk Ember printer or another 3D printer that can use SPARK technology and you have Print Studio installed you can enter Print Studio directly from Inventor and send your model to the printer for production.

-DAP

Inventor 2016 Updated Presentation Environment

The release of Inventor 2016 has seen a wide range of improvements and new features._One of the environments to get a refresh this year is the presentation environment. In years past the presentation environment, while valuable to design documentation and visualization, had some productivity limitations. From the what’s new in Inventor 2016 documentation Autodesk mentions the following points as the primary improvements to the presentation environment:

• Auto Explode command is updated
• Tweak command is redesigned with direct manipulation tools
• Creating and editing of trails has been simplified
• Component selection is improved

The first change that can be seen when starting a new presentation file is the Auto Explode command. Selecting Create View from the presentation tab presents some new options in the dialog box for creating an exploded view.

 

In the Explosion Method area of the dialog box, with the Auto Explode option checked, users can now control the auto explode to occur at just the top level of an assembly or to all levels of an assembly. The auto explode command is rarely successful at completing an exploded view without edits (as can be seen below) but these additional controls will allow more flexibility in creating that starting point for a presentation view.

In the two explosions pictured above the CORE.IAM subassembly is auto exploded as one component using the One Level option and as individual parts using the All Levels option.

There are new options in the Default trails drop-down list as well. Trails can be displayed automatically for All Components, All parts, Single or None.

All Components displays trails for subassemblies and top level parts included in a tweak. All Parts will display trails on individual parts regardless of assembly structure and the Single option will display trails for only one instance of a part or component being tweaked in an assembly.

Once you have an assembly model inserted into the presentation environment, whether it was automatically exploded or not, Auto Explode can be selected from the ribbon.

To activate the Auto Explode button, which may be greyed out, simply select the assembly node from the model browser on the left hand side of the screen. When activated the Auto Explode command will start a dialog box with the same auto explode settings available as in the Create View tool.

The Tweak Components command has also been revised with interface and functionality changes for better performance. The dialog box and triad previously launched with the tweak tool have been replaced with a mini-toolbar interface and an updated triad graphic. 

• The triad arrowheads are now selectable directly
• The Continuous Move button retains a selection set for a tweak after hitting apply
• The Part/Component filter allows a selection priority for tweaks in multi-level assemblies
• The Local/World drop-down will match the tweak direction triad to the respective coordinate system of the model.
• The Locate option is based on model geometry
• As with Auto Explode, Trails can be added with four separate filter options
• All Components, All Parts, Single and None
• Trails can be deleted by selection and added by selecting model geometry at any time during a tweak
• When adding trails the Full Trail/Trail Segments options will add a trail to individual tweaks or to a full sequence of tweaks on a selection respectively. 

Outside of the mini-toolbar interface the dimension parameter has been moved to a dynamic input field displayed on the model itself. This allows a user to type in a value without having to click the dimension box or to ignore the field altogether.

Finally, my favorite enhancement is the new ability to make selections during a tweak using the window/crossing window selection methods. Previously users needed to individually select components to be included in a tweak which slowed work significantly for all but the simplest assemblies. Now with the window/crossing selection ability and a selectable component/part selection priority the largest hurdle to quick explosions has been overcome.

With these updates in Inventor 2016, the presentation environment should be much faster and more user friendly when creating exploded views and animations. Geometry selection, trail settings and tweak operations have all seen improvements with speed and ease of editing in mind.

Inventor 2016 New "Import" Function

One of Inventor 2016 new commands is "Import".  It allows the import of various types of CAD files into the Inventor part environment and then allows the referencing of the geometry into feature sketches.  One of the key features of this process is that it creates an associative link to the imported CAD file.  If the imported CAD file in opened and edited in its native application then saved, the Inventor model will request to make all sketch geometry, created from reference geometry of the import CAD model, to update.  I only have access to AutoCAD so this is the imported CAD model I will demonstrate.  I have tried it with SolidWorks and ProE models and the importing and referencing of geometry works great, but I do not have either of these applications to test the update function.

The "Import" function can be found in two locations in the part environment.  These are shown below.

Selecting the function you are asked to browse and select the file you wish to import.  You can change the CAD type as desired but it defaults to "All Models".  If the file is an AutoCAD 2D file the next prompt is to select one of the part origin planes and then an origin point.  Normally I use the Center Point because I know I can move it later if needed.  The AutoCAD drawing appears and a notice about the associative link you are about to create.

Since it is highly unlikely that the AutoCAD drawing was places on the AutoCAD 0,0 point, you will notice that the drawing is also not located at the origin of the Inventor part either.  For AutoCAD drawings, there is a "Translate" function to help you move the AutoCAD drawing to the required location.  Of course it is not required to move the drawing, you can use the entities from where they came in.  Right click in the imported AutoCAD drawing in the browser and select "Translate".

A two directional/rotational (2D/R) icon will appear.  Two function options are also displayed in the head-up menu.

Select the "Locate" icon and then select any key point on the AutoCAD drawing to move the 2D/R icon to that point.

I made the Inventor Origin Center Point visible and then select the "Snap To" function of the 2D/R icon.  When I select the Origin Center Point, the AutoCAD drawing will snap to the point centering it in my part model.  You can use the Origin Center Point in the browser if you do not want to make it visible.  You can also select either directional arrow or the rotational ball to enter exact movement.  Select OK to finish.

 
Create a sketch on the plane your earlier placed the AutoCAD drawing.  A new "Project DWG Geometry" command allows you to reference geometry from the drawing. 

This tool has three options for referencing geometry.  The first one is "Project Single Geometry, the second is "Project Connected Geometry and the last is "Project DWG Block".

Using either of these tools will give you the familiar reference geometry your are used to in earlier Inventor versions.  Remember this reference geometry is associated to the original AutoCAD drawing.  I have placed a reference dimension on the hole to track associative changes.

  After extruding my model, I open the drawing in AutoCAD.  I change the hole in the plate to 5.0 inch diameter and same the file.

Returning to Inventor, I notice the AutoCAD drawing is showing the red lighting bolt indicating that a "Local Update" is needed.  After the update the model changes to match the AutoCAD drawing.

The associativity between the AutoCAD drawing and the Inventor sketch/model can be controlled in a similar fashion to a derived part.  Right click on the referenced AutoCAD drawing in the browser and select either "Suppress Link" or "Break Link".

The insert command, when used on other CAD files, has different functions but basically works the same way.  I will try to cover that one later.