Being Inventive

Virtual intersection not showing extension lines

You've created a dimension using the theoretical intersection point, but the extension lines that illustrate this point aren't showing up when you place the annotation.

Here is the dimension you want to create.

Fig 1: Expected virtual intersection

But you end up with below result. Why?

Fig 2: Virtual intersection witout extension lines

The reason is that the Origin Offset value (Dimension Style Setting) must be less than the distance between the intersection point and the nearest endpoint of a straight line.

If a dimension doesn't display the intersection point extension lines this means that your offset value is too large and you need to change your active dimension style and set a smaller origin offset value (on the Display tab).

Fig 3: Adjusting the origin offset value in the Style editor

This tip was graciously offered by Nathan.

Update:

Here is a video that shows the entire workflow on how to create a virtual intersection and how to adjust the extension lines.

 

Bob

 

How to add a spot face symbol to your drawings

We recently issued a hotfix to allow the use of custom fonts in hole notes. Right now the hotfix has been released for the Inventor 2010 Sp4 release only.

Note that thanks to this hotfix, 2010 users now have more powerful hole notes compared to 211, 2012 and 2013 users J.

But they will enjoy this exclusivity not for long. We plan to include the fix in the coming months in the service packs that we will publish for more recent releases.

Let me explain what this hotfix is all about so you understand the extent of its impact.

Without hotfix you are unable to add special symbols or character to a hole note unless you use the AIGDT font via the Character Map icon (see Fig 1).

Fig 1: Adding symbol from the AIGDT font via the Character Map

The AIGDT font suits most special symbol needs in the mechanical drafting arena, except for one particular situation.

It does not include a spot face symbol | SF | according to the ASME-Y14.5M-2009 drafting standard.

The spot face symbol is essential to distinguish a spot face hole from a counter bore hole.

Fig 2: Counter bore and spot face choices

Here is an example of a top view with seemingly two identical holes (if you just look at the hole notes)

Fig 3: Top view of two identical (?) holes

However when creating a section view, the holes look quite different.

 

Fig 4: Section view of the same holes

The hole on the left is a spot face hole and the hole on the right is a counter bore hole.

I admit that I artificially inflated the spot face depth to make it look more dramatic. But you will understand that there is a risk of misinterpreting the drawing by just looking at the top view and when no appropriate symbols are added to the hole notes. Here is where the above mentioned hotfix comes to the rescue. After applying the hotfix you can now select symbols from fonts other than AIGDT. You could even supply your own custom fonts.

If you include the spot face symbol as it can be found in fonts that are freely available on the internet (here is one example ASME-Y14.5M-2009 font), you get this result:

Fig 5: Addition of spot face symbol makes top view unambiguous

The only regret I have in all this is that we were not able to incorporate the same functionality in the style editor. This means that you won't be able to include the spot face symbol in a drawing template and that you will have to add the symbol on an individual note by note basis.

The other element to reckon with is that when you pack and go such a drawing to make sure that you also supply the special font to the party that receives your drawing. Otherwise they would not see the | SF | symbol.

But at least you have the power to create a hole note according to ASME-Y14.5M-2009 without waiting for Inventor to catch up with that standard.

Cheers
Bob

 

 

 

Cannot embed PDF files in a 64 bit version of Inventor

Please read this new technical article if you experience problems when linking or emdedding PDF files in Inventor.

Bob

Updating the Excel table in the drawing

You have inserted an Excel sheet in your drawing from menu Annotate > Table > General.

Without closing the drawing file, from Windows Explorer you open, edit the Excel file, close and save it.

In order to update the Excel sheet in the drawing with the changes you have applied without closing and reopening the drawing file, you just need to do the following.

Select the Table in the drawing browser or in the graphic window, right-click, Update.

Ale

Dimension of the internal circle of external threads in views

You have applied an external thread to a cylindrical part.

Then, you create the view of this part displaying and dimensioning the thread, but you want to know how Inventor calculates the dimension of the internal circle of the thread.

The calculation is based on the values in Threads.xls file.

For instance you have applied the ANSI Metric M Profile thread (M50x4, Class 6g) to a cylinder with a diameter D = 50 mm.

In this case the diameter d of the internal circle of the thread in the view is calculated with the formula below.

               d = D – [Major Dia Min (column H) – Minor Dia Min (column L)]

That is.

d = 50 mm – [49.465 – 44.642] mm = 45.177 mm

In case you apply a thread and its column L is empty in the Threads.xls file, as, for instance the ANSI Unified Screw Threads and the majority of the Pipe Threads, the diameter d of the internal line of the thread in the view is calculated with the formula below.

d = D – [Major Dia Max (column G) – Minor Dia Max (column K)]

Ale

Radian angular dimensions in drawings

You want to apply the angular dimensions in radian in your drawings.

You can set this in the model sketch, but not in the drawing dimension style.

Retrieving the dimensions from the model sketch in the drawing doesn’t help either.

The dimensions will be applied according to the active drawing style format.

By the way, if you want add the Radian values to the existing dimensions as alternate unit, you can do the following.

• Download and unzip this VBA Macro to your local drive.
• Menu Tools > Options > VBA editor.
• Expand the ApplicationProject so that you see the Modules.
• Insert a new module.
• Copy and paste the macro text in the module.
• Return to Inventor.
• Go to Tools > Options > Customize > Ribbon tab.
• Locate the macros by name in the left pane.

• If you want the macros to show up in the Drawing Annotate ribbon, select Drawing | Annotate above the right pane.
• Hit the >> button and set the Text checkbox.

Once you have completed the procedure above, you can open a drawing where you have already applied the angular dimensions according to the active style or apply them.

Then, in the Annotate ribbon, click on the command AddRadiansdToAngularDimensions and get the Radian values as alternate unit.

If you want to remove the Radian values, click on the command ResetAngularDimensions.

Ale

Components not visible in drawing views

You have created some views of your assembly and, in some of them, some components are not visible.

In general this can happen in views of large assemblies where small components don’t display.

Our development is working for fixing the problem.

In the meantime we hope you can find this workaround useful.

The workaround is based on the fact that the problem is not reproducible if the view is shaded.

• In the assembly, create or edit a color style, setting the opacity to 0.

• Create a new Representation View.
• In the assembly browser make a multiple selection of the components.
• Select the color you have created or modified from the Color drop-down menu for applying it to the components.

• In the drawing, edit the view where the components are not visible, apply the Representation View created and set the view as Shaded.

Actually the view will not display as shaded, but the components will be visible.

Ale

Export parts list to Excel in VBA

Apparently it is neither enough to provide BOM export to Excel interactively in the Inventor product as explained in this earlier post nor is it sufficient that we provide iLogic snippets to export the BOM to Excel via:

ThisBOM.Export("Parts Only", "fileName", kMicrosoftExcelFormat)

The crowd still wants to have a go at it the hard way by writing VBA code J
So let's give the crowd what it is clamoring for. "Panem et circenses" as the Romans used to say.

The VBA code that I came up with can be inspected and downloaded here.

A couple of conditions have to be met in order to successfully run the code (if these conditions are not met, you will get nagging warning dialogs anyway):

• First, add the Microsoft Excel Object Library to your VBA project by using the Tools > References menu in the VBA editor. This is a one-time operation.
  
  
  
• Make sure to have a drawing active in your Inventor session
• Close any open Excel sessions
• Select a parts list on the drawing before running the code.
  Important: the macro will expand the parts list automatically to all levels, before exporting it to Excel.

At runtime, the code asks you to give a full path to an Excel filename.

If the file does not exist it will be created.
If the file exists, it will be reused
The parts list will be created on a sheet called "BOM". In the case of an existing Excel file, all other sheets will be preserved.
If you want to put the parts list information on a different sheet, rename the string "BOM" in the first line of the code to something else.

    Const Sheetname = "BOM"

Here is a snapshot of a sample drawing parts list that was created with the "Structured (legacy)" option.

Here is the result in Excel on the sheet "BOM", after running the macro.

Hopefully I have now covered one more avenue to go from a BOM to Excel.

Bob

Remove trailing zeros of referenced parameters in leader text

You want to create a text with a referenced model parameter without showing the trailing zeros for the parameter value.

For instance, you want Value=70 instead of Value=70.00.

For doing this, in the Format Text dialog, you can set the desired precision before clicking on the “Add Parameter” button.

But if you change the parameter value from 70 to 70.5, in order to display the correct value in the leader text, you need to edit the text removing the parameter, change the precision and add it again.

So, if you want to display the maximum precision but without trailing zeros for the parameter value, a better workflow is the following.

• In the model, select the export checkbox for the parameter.

• Change the parameter property format removing the trailing zeros and unit.

• In the Leader Text, insert the parameter value as Custom Property – Model.

Ale

Insert COG in drawing tables

Here is a small little tip on how to include the center of gravity (COG) on your drawings.

I must admit that I narrowed the scope down a bit by looking only for the COG of sub-assemblies and not individual components.
With a bit of work, the procedure as explained below can be modified to suit also the display of COG of individual components.

My first thought was to use a parts list to display the COG.
But in situations where there are multiple instances of the same sub assembly (take an assembly pattern as example), each instance will have a different COG.
And as we all know, the parts list will roll-up all instances into a single row, which makes it useless to display COG on an instance-per-instance basis.

A better vehicle to display the COG is a generic table. Here is the workflow that I followed.

• Open up any assembly that contains sub-assemblies
• Run the macro that you can find here.
  The macro generates a CSV file in the workspace.
  The file has the same name as your assembly but with the extension .csv
• Create a drawing view
• Add a generic table to the drawing based on the CSV file
• Run the macro again when your assembly has changed.
  The generic table will update automatically once you activate the drawing.

Fig 1: a generic table with center of gravity data

The table in Fig 1 shows the result that I obtained on a not so randomly picked assembly J.
Note that the last two sub-assemblies have the same geometry but are obviously in a different position.

Enjoy!

Bob