Use 3D Solid Edges for Frame Generator Selection

Issue:
You use the Frame Generator tools in Autodesk Inventor all of the time, but you find that creating the base 3D sketch is tedious, time consuming, and doesn't always take edits well. Is there another way to do this?

Solution:
There are some times when a creating a 3D sketch is required, but often time it's helpful to know that you can use the edges of  a 3D base part to place Frame Generator members. When you select a part edge, Frame Generator automatically projects the geometry into the Frame Reference Model that it creates using the selected edges.

For instance you could create a basic 3D solid part model such as the one shown, and place it into an assembly file:

If you need more edges to use for the frame selection you can edit the base part model, and sketch on the faces of the solid:

 There are times where you might want to create a 3d Sketch based upon 2D sketch geometry. Here a 3D sketch is created and the 2D sketch is projected to the face pf the part to provide more edges to use in the frame. This is done using the 3D Project to Surface tool:
http://wikihelp.autodesk.com/Inventor/enu/2012/Help/3320-Show_Me_3320/3321-Show_Me_3321/3538-3D_Sket...

Often it's helpful to make the base part a clear color so you can see all of the edges to be used for selection:

 In order to prevent the base model from impacting the mass of your assembly, you can set it to Reference:

 Once you are finished selecting edges, you can just turn off the Visibility setting of the base part file, leaving only the frame showing:

Detailing Frame Generator Weldment Members Individually While Still Maintaining Assembly Features

Issue:

You have a Weldment Frame Assembly with assembly level features (cuts or holes in the parts made in the assembly rather than the parts themselves) and you want to detail each member of the frame individually and have it show the various assembly level features you've created. The problem is, the features do not exist in the part files. Is there a solution to this?

Solution:

There are actually a couple of solutions to this. The first one is the proper way to get the results you're after, but it's often overlooked. Even in a standard assembly weldment, many Inventor users overlook this functionality, and I’ve seen others go so far as to say it can’t be done (it can, of course). But when you add a fame generator sub-assembly into the mix,  fewer Inventor users connect the dots to get this all to come together. So I’ll go through the correct process here, but I'll also offer a workaround in case you're reading this after having already started out on a different path.

First off let’s make sure we understand how to detail members of a standard weldment assembly individually so that the preparation cuts and holes created in the assembly can be detailed too.

Here I have a weldment assembly made of two instances of the same block, Block100:

Because these blocks are the same stock part, if I need to create the hole in them I need to do it at the assembly level. If I tried creating this hole at the part level in each instance, I would end up with 2 holes in both instances (as well as all of the instances of this part I used in every other assembly). So this is a bad idea. Another approach is to save off a copy and start making “renditions” of this part (also generally a bad idea if it’s intended to be the same stock part number). 

So, to detail each part individually using the proper technique, I first create the hole as a weldment preparation feature. Then I create a drawing view of the weldment assembly, and go to the Model State tab of the weldment view and choose which member to detail. This is kind of like using a Level of Detail, but it's all set up for you automatically as a function of the weldment tools:

 

When you choose Block100:1 only that part is included in the view. Here is a drawing of the same weldment assembly file. Each view uses a different model state of the weldment preparations. You'll notice the browser displays which part(s) is shown:

Click to Enlarge

So that's the basics of detailing parts individually from a weldment assembly There is an entire chapter dedicated to Weldments in the Mastering Inventor books (hint, hint). It's because of this added ability to filter for just one part at a time, that I recommend converting Frame Generator sub-assemblies to weldments even if they are not truly going to be welded. Then you can create your assembly features in the Preparations folder and take advantage of the weldment drawing tools. But you have to do this in the Frame Generator sub-assembly NOT the top level assembly. To understand the issue more completely, let's first take a look at the anatomy of a Frame Generator assembly. 

When you created your first frame member you were prompted for a New Frame File Name and a New Skeleton File Name:

Here is a simple Frame browser structure:

CW-0323-01.iam = Top Level Assembly

Frame_Skeleton_CW-0323-01 = The user created part the frame is based on

Sub_CW-0323-01 = The subassembly that Inventor creates with Frame Generator. This is where the frame members reside (Sub_CW-0323-01.iam).

Frame Reference Model = The reference part that Inventor creates with the Frame Generator. This is where the copied reference edges used in the member placement reside (CW-0323-01_Skeleton.ipt)

Here is the same simple frame with assembly features created in the top level assembly (in this case it's been converted to a weldment).

This is not the preferred place to create these features, because we can't detail the individual members with the assembly level cut features if they are placed in the top level. Instead, assembly level features should be created at the frame subassembly level. 

In this next image the frame sub-assembly has been edited, converted to a weldment, and then assembly level features were created. The results are the same as before, but the features reside in the sub-assembly, which is required in order to use the Model State tab in the drawing views correctly.

When the features are created in the sub-assembly, you can simply create a detail drawing of the frame subassembly weldment (not the top level assembly) and then use the Model State tab to set the weldment Preparation option to look at each member of the weldment individually, just as you can do with any weldment assembly. Here is the frame sub-assembly in a drawing:

Here the Model State tab is being used to filter for just one part is to be used in the drawing view:

Here the individual frame member is being detailed, showing the preparation cut on the left. You'll notice the machining features (the circular cut and the chamfer of its edges) are not included, because those features are post weld features and are not part of the piece parts, but instead applied to the weldment as a whole.

 

That's all there is to it. As long as you convert the frame sub-assembly to a weldment, and then place your assembly features in that sub-assembly (and not the top level assembly), this works fine.

The Work Around

But what if you've already created your features in the top level assembly? 

If you've already created the features at the top level assembly, rather than the frame sub-assembly, you really should just take the time to recreate those features at the right assembly level. But if that would entail a great deal of work, you can use Level Of Details to suppress all of the parts you don't want in a view and then detail it using the Level of Detail in the view. (as with any workaround you might find flaws in it).

To do this first set the selection filter to Select Part Priority, so that you can reach down into the frame sub-assembly and select individual parts:

Next create a new Level of Detail:

 

 

 And suppress the parts you don't want to see:

Then suppress the welds if needed:

 Create a drawing view of the top level assembly, and use the Level of Detail:

There you have it. It would be ideal if you could just select the assembly features and demote them into the frame sub-assembly. But currently you can't do that.

As mentioned before, I recommend converting Frame Generator sub-assemblies to weldments even if they are not truly going to be welded. Then you can create your assembly features in the Preparations folder and take advantage of the weldment drawing tools.

Suggested Improvement (hint for Autodesk)

I think that this process could easily be improved by Autodesk if they were to make all Frame Generator sub-assembly files automatically have the same ability to "filter" for a single part file in the drawing view Model State tab, that weldments currently have.

If you'd like to suggest this to Autodesk also  you can use this form:
Feature Request For Inventor

Understanding Autodesk Inventor Frame Generator, Bill Of Materials and Part Numbers

Issue:

With the help of the Frame Generator you've used Inventor to successfully design a frame. The problem is in the way that Inventor creates a file for each member, and automatically sets the file name to the Part Number field. You've tried renaming part files but this seems to break more than it fixes. Isn't there anyway to get Frame Generator to cooperate and provide a Part's List that can be used for production?

Solution:

This is a bit of a process, but once you've done it a few times you'll get the hang of it. Also, keep in mind that you can set up a frame assembly template to have much of this done for you automatically in the future.

First off, for the most part you can forget about file names when using Frame Generator (FG) , and just let FG name the files as it sees fit. You do this by un-checking the File Naming checkbox as shown:

Typically the only FG files I set the name for are the frame sub assembly and the skeleton part file. Example:

UX950.iam = the container subassembly that all of the frame members will be placed in

UX950_ skeleton.ipt = the reference file that geometry is copied to. For instance when you select an edge to place a frame member, that edge is copied into the skeleton part file.

Here is a simple example I'll use to explain this better. As you can imagine there are many members of the frame that are identical, and ideally we'd like to have those members share a common part number.

Here some identical frame members (the stair treads) are shown in red.

Here the railing members are color coded to show the common members.

The first thing to do is edit the Bill of Material (BOM). Go to the Assembly tab and click the Bill of Materials button to bring up the BOM editor. 

Next, let's talk a bit about the quantity columns in Inventor.

Inventor has 4 of them, Base QTY, Item QTY, Unit QTY and QTY. You can use the Choose Column button to add them to the BOM for review (this doesn't impact the parts list on the drawing).

Base QTY = length of the part (reads the G_L iProperty from the part file). Can be changed in the BOM editor.

Unit QTY= the same as Base QTY, is read only and can't be changed in the BOM editor.

Item QTY = counts the number of parts in the assembly with the same part number

QTY = Base QTY x Item QTY

To add these columns to the BOM editor you can drag and drop columns to the BOM grid. Drop the item on the header row to add. Drop it anywhere you see the black X to remove it.

Okay, let's get started. I use the Add Custom iProperty Columns button to create custom columns in order to adjust the BOM to my needs. These custom iProperties will be pushed down from the assembly and written to the part files.

I'll add two new iProperties, one called Job Number and the other Mark Number.

Once added to the BOM grid you can enter a value for the Job Number and then use the Fill function to copy it to all of the cells below it. This writes the Job Number to each file shown in the BOM.

Next I'll use the Create Expression button to create an expression in the Part Number cell of the first member in the frame.  

I like to create a temporary expression using the Job Number, Stock Number, G_L and Mark Number properties. Even though the Mark Number is currently empty.

I then use the Fill function to copy the expression to all of the cells below it, just as I did when adding the Job Number. It is at this point, that I like to check and make sure the reference part that I used to select edges from for the frame is set to be Reference, so that it does not show up in the structured BOM or impact the mass properties of the assembly.

Once that is done I switch from the Model Data tab to the Structured tab and enable it if needed.

You'll notice that in the structured tab the parts are grouped by part number. This is controlled by the Part Number Merge Settings. I want this option Enabled.

Because the frame members are being merged by Part Number, and the Part Number consists of the Project Number, Stock Number and Length (G_L), I'm able to select the members with the same length as a single line item, and see them highlighted in the model. Here the tread channels of the ladder are selected:

Since all of these are the same, with none of them being mirrored or having a different hole configuration, etc. I can apply the same Mark Number to them. Adding the mark# to the Mark Number cell, automatically adds it to the Part Number, because of the expression in the Part Number cell.

I then do this for each of the common member groups as needed.

But then how do we separate out the members that are the same stock profile and the same length, but are right and left mirrors such as the sides of the platform shown?

To do this select the row, and then click the Show button at the top of the BOM editor.

This will expand the group and allow you to add Mark Numbers to each row.

For some reason, the members aren't highlighted on screen when doing this. So if the mark# needs to be something like P1L (for left) and P1R (for right) I'll typically just mark them both as P1 at first, and then flip back to the Model Data tab and determine which is the right and which is the left, and then adjust the mark numbers as needed.

Once the mark #'s are set, use the Clear button at the top of the BOM editor to collapse the group.

Okay, so once I have the mark numbers set for all of the members, I'll then adjust the part number expression to use only the Project# and Mark#.

Here the top cell has been adjusted and I used a dash to combine the project# and the mark#.

Then I use the fill function to copy the expression to all of the other part number cells.

Then I'll click on the Part Number header in the grid to sort by part number. You can also use the Sort button at the top of the BOM editor dialog box.

Once sorted, I'll use the Renumber button to update the Item numbers.

And then I'll add expressions to the Description field to adjust them as needed.

Here is an idea of what the BOM would look like when done. Notice how the quantity columns reflect different values now. The icons on the far left with the different length bars and an arrow, indicate the merged rows.

And finally, I'll use a balloon style that calls the Part Number and the Item QTY properties as shown:

Click to Enlarge