Top 20 Tips and Tricks in Inventor Professional

JOHNSON SHIUE: Hello. Welcome to AU class "Top 20 Tips and Tricks in Inventor Professional." My name is Johnson Shiue, your speaker today. This session contains 20 plus useful workflows in Inventor you may or may not know. Let's get started.

This brief introduction of myself. I live in Michigan with my family. I got a degree from National Taiwan University and Purdue University. I joined Autodesk in 1997 as a junior QA member. I work for Autodesk-- work for Inventor for 22 years. And travel around the world, and you can see a long list of countries.

And credits. The presentation was made possible by Autodesk. Special thanks to Autodesk D&M team, Inventor product team, and Inventor user base for their knowledge and encouragement. Sincere gratitude to my family and the late Dr. Joseph T. Pearson.

A brief history of [INAUDIBLE] Inventor. Inventor was first released in 1999. It contains Parts, Assembly, and Drawing environments. And gradually, we added more features. As you can see, in R6 up to R8, we got iPart, iAssembly, iFeatures. And then R9 to R11, we got iAssembly and other specialized components workflows. And 2010 to 2016, we got Multi-Solid Body and Sheet Metal, further enhancements and iLogic. In 2017 to 2021, the focus was on AnyCAD and also performance and stability enhancements and modernized UIs. And for recently, we add more workflows and model states.

And the topics we cover today will be in Part, Assembly, Sheet Metal, Drawing AutoCAD-related workflows. Import/Export, followed by Q&A.

The tips. The first command we want to cover is called Delay Face. Delay Face is available in Part environment. It can delete selected faces from a solid body or a surface body. It turned a watertight solid body into a surface body. It can be used to simplify geometry by removing detail faces.

The Delete Face can delete lumps too. A lump is basically a group of surfaces-- a group of faces. The lump-related workflow will be covered in later slides. That's just watch a short video showing the workflow.

Here is a shell box. And then you can select those wrong faces and delete it. Now, the part becomes a surface. The solid becomes a surface part.

And let's repeat the same process by turning on the heel command. So like those round faces, and you see the edges are recovered because of the other adjacent faces re-intersect.

Next, we're talking about Sheet Metal Double-Thicken-Intersect technique. It's very common to create a non-perpendicular cut in a sheet metal part. The resultant side faces may not be perpendicular to the sheet metal faces unless the cut normal option is used.

This so-called Double-Thicken-Intersect technique ensure the edges and faces on both sides of the sheet metal part to be consistent. And it can also be used within unfold and refold. Let's watch the workflow.

Here is the raw sheet metal part with the circular bar passing through. As you can see, the cut side faces are not perpendicular to the sheet metal faces. So they are not perpendicular to the sheet metal faces. They just simply follow the contour of the bar.

And in flat pattern, you can see it's more apparent. The cut faces are not perpendicular to the flat pattern body. If you zoom in closer, you can see the back edges. This kind of flat pattern will lead to manufacturing confusion and manufacturing difficulty.

So start second command. And select the intersect option. And you select a sheet metal face and set the distance to the sheet metal thickness. You may have to do it from outside just to ensure the side faces are perpendicular to the sheet metal face.

Now, go to flat pattern. And you will see the cut faces are perpendicular to the sheet metal faces now. And the edges are all aligned. You cannot see the back edges.

Next, we will talk about iFeatures or Extract iFeatures. iFeature has been around for a long time, but the process of extracting can be tricky. So basically, iFeature is a group of features to be extracted from a part. And then you can insert the iFeature to another part.

Sometimes it can be frustrating because of certain feature or geometric requirement. Here are some best practices for you to remember, then you can successfully extract iFeature. Do keep future dependency simple and easy to understand. So for example, a feature C depends on feature B and depends on feature A. So the dependency is more linear and avoid any cross-feature dependency.

An edit the sketch coordinate ensure predictable orientation. And then share the sketch whenever possible. And lastly, test the iFeature on a different placement plane to ensure it can be inserted successfully in other parts.

Things to avoid. Don't project origin geometry or face loop to a sketch. And do not use vertical horizontal fixed constraints because these constraints can rely on the orientation in the part. And that condition may not be the same as the new target part. And use perpendicular parallel constraints instead because they will be relative to other sketch geometries. And 3D sketch is not supported, so avoid using 3D sketch in the source feature you like to extract.

And following the prior discussion, here is the workflow on how to edit 2D sketch coordinate. Event 2D sketch coordinate is dependent. It's determined by the selected planar face loop. When a loop consists of string segments, Inventor may choose one segment as the reference for the x-axis.

Usually, the sketch origin point may snap to one of the endpoints, depending on the geometry. The sketch coordinate placement may not be desirable. A simple workflow here can help you to relocate the sketch coordinate to the desirable position and also align to the desirable orientation. And you may need to flip the coordinate direction, if necessary.

Another option is to create UCS. And that create a sketch on UCS plan will give you more predictable result. Let's take a look at the workflow.

So try to create a sketch on a small rectangular face on the right-hand side. And you will see you right-click on the sketch, and that it's like add a sketch coordinate. And you see the sketch coordinate is aligned to that face. Now, you relocate the origin to the power origin and realign the edge, the x-axis to the edge or to an axis or to another sketch created before this sketch. Now, you relocate it.

Next, we will talk about different ways of creating organic shapes and a stylish shape. In Inventor, it's basically four-- there are four different commands to do that-- loft, sweep, boundary patch, and freeform. For sweep, basically, a sweep is a profile or a volume goes along a predefined path. Its orientation can be controlled by a guide surface, or the profile can be scaled by a guide rail.

The profile is better placed at either end of the path, not in the middle. The resultant shape is universal in other CAD system also. You can recreate the same exact shape in other CAD tool by using the same condition and same geometry input.

Loft. Loft is a smooth shape passing through sections. The progression of the loft can be controlled by the sections and the spacing between sections and the rails. The shape may be CAD work dependent. You may not be easily recreate the same loft shape in other tools because of the loft algorithm is proprietary.

A freeform. Inventor freeform is based on the Tspline technology. And Tspline is a type of subdivision surface. Its accuracy is obtained by subdividing the surfaces.

The shape is always smooth. There are no sharp edges. Certain constraints can be applied. For example, like symmetry or like matching edges. And you edit the freeform by pulling the vertices and edges.

Boundary patch. It's a smooth surface fit over a closed boundary. If an open loop is selected, the untrimmed surface will be created. And you may use guide curve edges or vertices to control the shape.

Here is the video showing the variation of these surfaces. There are five surfaces in the model space. The first loft is created by sections. And you will see there are two circles and four section rails. The result is relatively smooth.

The second loft is by center rail. You have two sections, two circular sections, and the rail. It's quite similar to sweep. And this sweep is by one profile following the path and the guide rail to control the sections. And the boundary patch is created by two circular edges and fitting over the two surfaces.

And the freeform is similar. And that's how they look like in zebra analysis. So when we zoom in closer, you can see the sweep guide rail surface gives the best symmetric result and the most smooth result. Other type of surface will give you a little bit of variation here and there.

Next, we will talk about the predefined features in Inventor. Basically, Inventor has primitive workflows or placed features workflows and Insert iFeature workflows. And primitive is available in 3D Model tab. And place features, it's from Content Center. And you can also predefine features by-- you can also define your own features by publishing in Content Center.

And then you have Insert Features from the iFeature Catalog. And each of these require selecting a plan of reference. Let's see the workflow.

The primitive, you got box cylinder, sphere, and torus. The command is enabled in Ribbons. You just do like a point of reference. And then the cylinder will be created. You don't need to create any sketch manually.

And then place features from Content Center. These predefined features are all in Content Center library. They are categorized by their shape and also by the units, English or metrics. And here is a set of iFeatures punch tools predefined in Inventor. And you can build your own library by extracting iFeatures.

Unwrap. Unwrap was added to Inventor 2020 release. It can flatten almost any face, solid body or surface body. Internally, the command convert the selected body faces into mesh and flattened the mesh. And then you can use certain straight edges to align the flattened surface.

And lastly, Inventor fit a planar surface over the mesh, and convert the mesh back to the Brep body. The process does not consider material deformation. And also, it doesn't consider the sheet metal k factor. It's best to use for estimating an area or extent of fabrics. Let's see the workflow.

This is the headrest part from the car seat sample. Start Unwrap command. And you can select the faces. The preview may appear at a designated place, either at the part origin or attached to the coordinate system on the body.

You may select the linear edge to align the flattened face. And such realignment can lead to shape change as you can see. So the resultant flattened surface, it's not accurate. So you may have to iterate. And this is best to use approximate an area required to cover something.

Next, we'll be talking about STEP files, how to downsize the files. In Inventor, parts and assembly can be exported to STEP. STEP files tend to be bigger than the source IPT or IM file.

And basically, what contribute to the size is the number of unique definition and the geometry complexity and the spline fit tolerance. Inventor STEP exports spline fit tolerance is set to 0.001. And if you increase the tolerance, meaning you loosen the tolerance, actually, you can help decrease the file size. And the range is between 0.01 millimeter to 0.0001 millimeter. And I'll show you a workflow and see how that value impact the file size.

And in an assembly STEP file, you do want to reuse components. So that will reduce the file size also. And lastly, you want to simplify the geometry. So the simpler geometry is, the smaller the step file become.

Lastly, this may not be related to the file size. But oftentimes, users may not be aware that they use duplicate components, duplicate files in the folder. Although, Inventor can handle duplicate files, but the neutral file format, like STEP, cannot. So it can create confusion. So always make sure your component definitions are unique. Let's see the workflow.

Here is the car seat sample. I have already exported the car seats in different spline fit tolerance. And you will see the result. So from 0.01 millimeter to 0.0001, and you can see the tighter the tolerances, the bigger the files.

Cyclic AnyCAD reference. So AnyCAD workflow was first introduced in 2016. It can help link a non-Inventor CAD file associatively. When there is a change in the source CAD file, the Inventor will be aware and update the geometry accordingly. This workflow primarily allows the model geometry to transfer from one CAD system to Inventor.

But it also enables a semi-cycle. And you may export an assembly or a part to STEP. Then use any CAD reference workflow to link it back. It's kind of like deriving oneself.

The usage of workflow is when you build certain geometry or component within the model, but you want to reference only portion of the model in a different place. The interesting thing about this workflow is the ability to control when to update, when the update happens, and whether or not a change in the source is needed to propagate them.

So let's say you have your source Inventor assembly or part. And you can export it to STEP. And then you can use any CAD associative reference workflow and insert it back to the same assembly. Let's see the workflow in video.

The test station. Let's say you want to reference only the frames, but the frames belong to two different sub-assemblies. So you create a design view just capturing the frame member scattered in different sub-assemblies. And then you can export it to STEP. And later on, you can link it back for reference purpose.

Now, you go back to your original assembly. But you link your exported sub-assembly. Then you can start building your component based on this self-exported and self-imported sub-assembly. And when the frame size changes, you can export it again and then bring it back. And you can automate the process using iLogic.

Keep z-axis upward. By default, Inventor sets y-axis pointing upward to the top. This allow a user to design on xy plane when viewing the front of the model. However, in many industries, the z-axis needs to point up. Here are the steps to change the ViewCube Orientation and keep the z-axis up.

Set up ViewCube options and redefine the ViewCube front, top, home. And make the origin planes visible. This will avoid ViewCube rotate when you create a sketch. An optional step is to redefine the part design views. The predefined part design views need to be updated accordingly. Lastly, you have to apply the same change to assembly and parts and templates. Let's see the workflow in video.

By default, the y points to the top. Now, go to Tools, Application Options, Display, ViewCube. And set the desirable default front and top. In this case, you want to set it to xz front, but the top is set to xy.

Then go to ViewCube menu and reset the front. So now, the z points to the top. But you would like to reorient the ViewCube and then redefine the home. And save the change.

Also, you want to make the origin planes visible. If you don't, you see the ViewCube will switch back to y up. Because of the visible origin planes, the ViewCube will no longer rotate.

The tricks. In the prior section, we talked about lumps. So what is the lumps? User often wonder the difference between lumps and bodies.

Geometrically, they look the same. They are basically just separate groups of faces. But in Inventor, their internal definitions are quite different.

When the two bodies overlap, they don't join. But when two lumps overlap, they join automatically. This allows geometry patterning to work more efficiently because all the lumps can join in one operation as opposed to combine individual bodies.

And we hear user asking, how do I separate lumps into bodies? Here is the workflow. First, you need to find out how many lumps you have. And then you pattern the bodies with the multi lumps to the number of lumps. And then use the Delete Body Lumps selection to remove the unwanted lumps. Let see an action video.

In this case, there's a body with two lumps. I'll use the direct edit to show you the lumps will join if they overlap. So we move the cylinder closer to the box. As you can see, the faces merge. So now, there is one lump, but there is one body.

So how do we separate the lumps into bodies? First, you want to pattern the body. This body has two lumps. So you want to pattern two instances, but keep the spacing to zero. So essentially, the body is on top of the body.

Then, you hide one body and remove the unwanted lumps. And use Delete Face Lump Selections. And repeat the same process on the other body.

Now, you have two separate bodies. Each one has one lump. If I move the body closer to the box, you will see they don't merge.

Next, repair bodies. Inventor has a dedicated repair body environment in the part. Mostly, it can be used to fix bad geometry on an imported body. And whether or not the repair process can succeed largely depends on how bad it is.

There is also another environment offering similar workflow. It's called construction environment. And people always wonder what's the difference between repair environment and construction environment. It's about the data's persistence.

The body geometry in repair environment is always there. It can be referenced or consumed by other features in order to create a new feature. But the body geometry in construction environment cannot be referenced or consumed by any parametric feature. It's more like raw data.

So in some cases, the repair workflow may not be enough. The bad geometry needs to be deleted and recreated. This cannot be done in construction environment. Some users even report that the roundtrip IGES translation may help fix up bad geometry. This may have something to do with Inventor IGES translator's ability to heal geometry, but it may work for some cases but not all cases. Let's see an example of repair body workflow.

The first thing you need to do is you want to move the problematic geometry to repair environment and then run find errors. It depends on the error type. Different commands are offered. In this case, it's the intersection. There are bad intersection faces in this body.

So use the Intersect Faces command to remove unneeded faces. And then you want to stitch the surfaces. You always want to start from the smallest tolerance and gradually work the way up, gradually loosen the tolerance. And in this case, you eventually get to a good solid body.

Sketch blocks. Inventor 2D Sketch allows user to create sketch blocks. Just like AutoCAD block references, a sketch block is like a rigid body. It's parametrically driven the degree of freedom within the sketch geometry is to remove. The entire block moves together. It can be copy, paste, derived, pattern, and mirror. And nested blocks are allowed, just like in the AutoCAD block reference.

Instances or occurrences are also allowed. And make component commands and make part commands can help you push the blocks into individual parts in an assembly. Let's see an example of sketch blocks.

The video shows the difference between regular sketch geometry and sketch block. When the sketch is copied and pasted, the parameters are all replicated. Essentially, the new copy of the sketch geometry is independent from the source.

Now, let's say [INAUDIBLE] sketch block [INAUDIBLE]. So you select the geometry to define a sketch block and define an insertion point and give a name. And you can insert as many sketch blocks as you like. These are all instances of the sketch block. And you can also edit the sketch block. And once you change the dimension, all blocks update.

BOM. Use BOM as an assembly control panel. Inventor BOM table is part number-based. The components sharing the same part number are merged to the same role. The table can be used as a control panel.

And most of the properties can be seen and added on the table. The component can be opened from the table. Model data, structure, part only views are available. The model data is always there. It shows the assembly structures fairly similar to a browser, except the same part number roles are merged. The column widths and the columns in the column definition can be saved in an IAM file or an IAM template. The BOM table can be exported to a predefined template.

We use the brewing stand sample to show this workflow. You can add any property column to the table so you see each component's status more clearly. You can change the BOM structure property. You can change the structure view from one level to all levels so you can see the nested components.

In the arrow, the arrows means those components were promoted from lower levels. In part only, structure tabs can be enabled or disabled. And this is the option to control if part number rows are merged or not. From 2023, there is an option to remove or hide the zero quantity role. And you can export the BOM.

iLogic. Inventor iLogic was available in 2021. Ever since, the iLogic adoption has increased dramatically. More and more people are using iLogic. Please note that this is not an iLogic class. There are many wonderful iLogic classes at AU. Please look into those for more detailed information.

This particular slide is about how to use iLogic right away. If you don't know about iLogic, I will show you a very simple workflow. And it will be really helpful.

All you need it's a simple rule at the top level assembly. It helps you manage your parameters efficiently. You will be able to change parameters in all components. Without iLogic, you will have to link or derive parameters or use crossbar project workflow. Let's see it in action.

So in this case, there are two parts-- the green box on the left and the purple box on the right. So I want to use the green box to drive the purple box. And we can create a simple iLogic rule in the assembly. And you capture the parameters from each component.

And then you find the related parameters and set up their relationship. Just these two lines allows you to drive-- to use the green box to drive the purple box. Now, whenever the green box changes, the purple box will update also.

The beauty of this workflow is that the relationship is managed outside of the boxes. The parts itself, they don't know such relationship. iLogic build a bridge to make it happen in the hosting assembly.

Default drawing dimension types. In Inventor, there is only one common dimension in command in drawing environment to create linear, angular, and radial dimension. There is a way to configure the default dimension types for linear, diametric, and radial. This option is in tools application options and drawing. It's not in the style editor or document settings. Let's see it in action.

We got a rectangle in the circle. So like the vertical line, it gives you the distance vertical dimension. And if you select a circle, it gives you the diameter dimension, diametric dimension. And such default is based on these options.

So you can go to Application Option and change the default dimensions. And you will see the difference. Now, by selecting the upper lines, actually it gives you the linear diametric dimension. And also, you can see the circular dimension is changed.

Copy model properties. Inventor Drawing allow a user to create drawings, drawing views for one component or many components. Some users prefer one drawing file per model. So each drawing goes with a part or an assembly.

This means one drawing only represents one part or one assembly. Naturally, you would like to have the drawing properties mapped or in sync with the model properties. Then, the copy model property works well becomes really handy in this case.

To do that, you will need to go to Document Settings. You can select the Custom Model iProperty Source and also select the property you would like to link from the model. Let's see it in action.

This assembly has a few custom iProperties. These iProperties don't exist in the drawing file yet. So if you go to the iProperties, you will see the model does have some custom iProperties. For example, let's focus on the cage. And you go to drawing, and if you look the same, you couldn't find it.

Then you go to Document Setting and select the Custom iProperty Source, which is the assembly. And then repopulate the cage to the list of iProperty to copy or link. Now, once you place the drawing view of that assembly, the iProperty is copied or linked.

If you change the source iProperty value in the assembly and in the drawing, it will be updated. But you have to go to Manage and click on Update Property button. And that property will be updated. So in this dialog, there's additional workflow only available in 2020 4.1 and later. You'll be able to copy and paste iProperties from one file to another.

Now, we are moving close to AutoCAD-related workflows. The DWG Underlay. Traditionally, AutoCAD 2D geometry has to be translated and converted to Inventor 2D sketch. Depending on the complexity of the 2D geometry, the process can take a long time. The resultant 2D sketch may be too massive to control, to consume in Inventor.

DWG underlay workflow will help in this case. You can link the 2D DWG geometry as a transparency-like object in an Inventor Part or Inventor Assembly. Project the DWG geometry selectively.

When the source DWG changes, the Inventor sketch will update. One caveat is AutoCAD DWG points are not included. And the 3D geometry cannot be projected at the moment. Let's see it in action.

So here is the Inventor Part. So you click on Import button and select DWG file. So the DWG geometry is linked to the Inventor file immediately. Then, you use Project DWG Geometry command and select the geometry you want. And you can immediately create features.

And you can go back to AutoCAD and modify the 2D geometry. So for example, you want to move the whole slightly lower and finish editing the block. And save the change in AutoCAD. Go back to Inventor. Inventor is aware of the change. And click on Update, the whole updates.

Draft Views. Inventor Drawing views are mainly based on model geometry. It's like a camera looking at the virtual model from a distance at an angle. Without a model, there is no drawing view. However, Inventor does allow a user to create a drawing view from 2D sketch, just like AutoCAD. And such a view is not associated with any model geometry. So some people say it's so-called AutoCAD-like view.

The view can be dimensioned and annotated accordingly. But because of lack of model, the scale is assigned by the user. The dimension on the paper should be in sync with the sketch dimension regardless of the scale. But the line type and line color can be tricky.

The drawing sketch line type can be modified on a per line basis. But in the draft view, the line type can also be altered as a whole on a per layer basis. Let's see it in action.

How to recreate an AutoCAD-like view in Inventor. You create a draft view. You can simply copy AutoCAD 2D geometry. And go back to Inventor and paste it. It's a view without any model association.

The next three slides will be related to AutoCAD. These workflows are AutoCAD workflows, but they work side by side with the Inventor very nicely. So AutoCAD-- many users don't know that AutoCAD can create associative drawing views to Inventor components. Essentially, you use AutoCAD to create Inventor Drawing views without using Inventor Drawing environment.

The AutoCAD command is called VIEWBASE. The nice thing about this workflow is when the Inventor model changes, the AutoCAD will update the drawing views accordingly. Essentially, you use the AutoCAD as the drafting tool.

The next command is called EXPORTLAYOUT. EXPORTLAYOUT helps convert drawing layouts from a paper space to model space. This is particularly handy for Inventor drawings. And lastly, AutoCAD has the ability to link to Inventor components and place such components in model space. And when the Inventor model updates, AutoCAD model space will update accordingly. Let's see it in action.

VIEWBASE. So first, you have to select a template and then use VIEWBASE command to select an Inventor component. Then you simply place the view. It's an associative drawing view onto the layout. And then you can utilize all AutoCAD drafting tools to annotate the view.

EXPORTLAYOUT. So you have an Inventor IDW file, and you like to export to AutoCAD. Sometime you may not get the desirable result. So you can simply save the IDW file as Inventor DWG file. AutoCAD can open Inventor DWG file. Then open the DWG file in AutoCAD. And then export the layout to model space. The result is 2D geometry in model space.

Next, Inventor Link. Again, select a template in AutoCAD. And you can select an Inventor component, parts, or assembly and place it in the AutoCAD model space. You can either edit the geometry here or create your own view based on the 3D geometry.

Display mass properties in graphics window. This is a nice workflow discovered by user. You can add the mass property in the graphics window. You first want to ensure the physical property is up to date, or it's always up to date.

And in the Annotate tab, you can use general notes, and then add a mass property or any property you like. And then it will be always in sync. Let's see it in action.

So first, you want to check if the mass property is up to date. You can click Update to update the property and save, or go to Application Options and make sure the physical properties are up to date and save. So whenever you make changes to the files and save, the mass property will be computed automatically.

Now, you simply add a general note to the graphics window. Select the place to place it and include the mass, in this case, also the part number. Now, you see the part number and also mass property shown in the graphics window.

The bonus. There are additional workflows to cover like ipj file. So basically, ipj file is a text-based XML file. So, although you can use Project Editor to change the option, you can simply use Notepad to edit the file and save it accordingly. But be sure you want to keep a backup of the file. So if you somehow make a mistake, you have something to refer back to.

Enable relationship redundancy analysis. This option can be found in application option. This option does literally the name implies. Basically, it finds all the duplicated constraints that do not reduce the degree of freedom. And then, Inventor mark it with an exclamation mark.

Inventor assembly does allow redundant constraint to be created for ease of use. But excessive redundant constraint can lead to poor solve result and poor performance. It is better to keep the assembly constraint free of redundant constraints.

Turning on the option has benefit more than just removing redundancy. When this option is on, Inventor Assembly Constraint Solver will solve more thoroughly, as opposed to solve locally. There could be minor performance degradation, particularly in a larger sample, but it should not be noticeable in modern powerful PCs.

The solve result is more accurate. So as a result, the new degree of freedom analysis, the black dot, requires this option to turn on. And after the option is turned on, you need to use Rebuild All to recompute once.

Rebuild All. People often ask, why do we need this command? The existence of rebuild all actually means something doesn't work correctly. It shouldn't be needed in the first place. But there is a subtle difference between rebuild all in an assembly and rebuild all in a part.

In an assembly, the rebuild all compute assembly parameters, assembly constraint, assembly features, assembly sketches, and well-beings and adaptive features even in the part and graphics. But in the part, the rebuild all computes all the part parameters, part feature, part sketches, and graphics.

So as I mentioned earlier, if everything works correctly, rebuild all should never be used and should never be needed. And also, rebuild all should never lead to any change, except the file needs to be saved. In drawing views, when the models have been rebuild all, the associative drawing view will need to be recomputed and updated and then saved.

Model states. What is model states? Model states are available in Inventor 2022 and later to replace OLD.

It allows users to have variations in parameters, properties, feature suppression, or component suppression and different BOM. The variations are captured on model state table, quite similar to iPart ISM. The difference is in each model state, there is a mini file within the IPT or IAM file, as opposed to separate IAM or IPT files in an iAssembly or iPart.

When do I use it? You may use model state to document machining states. So there's geometric difference or manufactured states, like the bend table, like bend sheet metal bends, or changing positions or in different configurations. And what are the limitations in model states? Model states are self-contained and managed by each model state table. Cross-component workflows are not supported. So adaptive derive only works in one model states.

Specialized components like voltage connection, cable and harness, fringe generator, content center, tube and pipe do not support model states. If you want to obtain the old LOD behavior, the closest workflow is using design to hide, as opposed to suppress.

And how do I use iLogic with model states? iLogic rule should not constantly change model state table. iLogic rule, it's best used to check for changes applying to all model states, the so-called factory scope.

We are reaching the end of the presentation. In summary, we have covered quite a bit. In parts, we talked about delay phase, insert iFeature, change schedule coordinate, and surface modeling unwrap. In assembly, we talked about BOM, iLogic parameters management, assembly relationship, and cyclic AnyCAD rebuild.

In sheet metal, we talked about double-thicken-intersect, sketch blocks, and unwrap. Import/export, we talked about cyclic reference, repair bodies, and how to keep z-axis up. In AutoCAD, we talked about view-based export layout, Inventor link, and doing underlay. In drawing, we talked about copy model properties and drawing dimension default and AutoCAD workflows.

If you have further questions, please feel free to send me an email. And here is the QR code to my email address. Thank you. Thank you for listening to the lecture. I hope you enjoyed it.