Setting Inventor Sketch Initial View Size

Early on in my use of Inventor I found the default size of the first sketch of a new part very annoying.  I researched it and found the setting under Document Settings that was suppose to control it.  On the Modeling tab you will find the settings for the "Initial View Extents".  I normally work in metric measurement so I set it something slightly larger than a common part size.

After this was added to my part template, I thought I was ready to go.  Well something else was controlling the initial view extents because my first sketch of 200 mm x 180 mm did not fit the screen.  Experimenting a bit, I found the settings for the initial view extents would be respected if I first selected the original sketch plane from the origin folder then right clicked to create a new sketch.

It would also work if I set the Sketch on new part creation located on the Part tab under the Application Options to a set origin plane. 

Both of these solutions defeated one of the great features of Inventor which is to select the original sketch plane during the first sketch creation.  Upon further study I determined that the original size and the "Auto-Resize" option for each origin plane was the problem. 

I opened my Inventor metric part template and created a rectangular sketch on each origin plane 30 mm larger than my initial view extents settings, in other words 280 mm x 230 mm.  I then made each origin plane visible and enlarged it to match the sketches.   I turned off the "Auto-Resize" option for each origin plane.  Last I made each origin plane invisible, erased my three guide sketches and saved the template.

The next time I used the part template, selected the "Start 2D Sketch" command and selected my sketch plane I was pleased to have room to fit my first sketch without having to zoom out to see it.  Actually the initial view extents is much larger than you specified due the fact Inventor allows space around the initial origin planes, so you may want to adjust your dimensions during setup.

It really does not matter because Inventor will automatically size the display of the first model when you select the "Home View".

This was my solution to setting the Initial View Extents, if there is an easier way to configure Inventor to do the same thing, please let me know.

Saving Fusion 360 Files Directly to Inventor

As Autodesk Fusion 360 becomes a more popular design platform the ability to transfer files directly from Fusion 360 to Autodesk Inventor will be necessary.  Currently inside the Fusion 360 application you can only export files to a CAD neutral format.

These, of course, can be used in most any version of Inventor.  There is a way to export both Fusion 360 assemblies and parts directly in to Inventor.  This is done from your Autodesk A360 project where your Fusion 360 files are stored.  Select the file you are going to export and select the export icon.  From the dropdown select Inventor 2014.  If you are currently using an earlier version of Inventor, you should stop here and use one of the CAD neutral formats.

 

Once selected you will receive a message regarding the creation and delivery of the file(s).  If the file selected is a Fusion 360 assembly, you will received a zip file in the email containing the assembly IAM file and all the related IPT parts.  If the file is a single part, it will be emailed as an IPT.

 

After receiving the email and downloading the attached files you will have to unzip them if it was an assembly or save the part to your Inventor project workspace.  Once open in Inventor, the assembly had many of the characteristics of a CAD neutral format.  The assembly parts are not constrained and they are dumb solids if they are edited.  If you are using Inventor 2016 or 2017 you do have a vast array of commands to edit solids so it is not that bad to make simple edits.

 

 

 

Just another way to interface between the two applications.







Inventor - New Sketch Look At Behavior

When a new sketch is created on a face of an existing part, the program will align the selected face normal to the view.  This is the default behavior applied when the program is installed.  This rotation may be prevent by removing the check mark from the following setting on the Sketch tab in the Application Options dialog box.

Assuming this setting is checked, there is another setting that will limit the rotation of the existing model view required to place the selected face normal to the view.  When Inventor is installed, the following setting, located on the Display tab of the Application Options, is set.  This setting will rotate the view by enough rotation, not only to make the view normal to the sketch plane but will also align the horizontal and vertical axis of the current plane.



 

Below is a short video showing this rotation.  Note the amount of rotation required to align the dark horizontal axis with the view.

 



 

Many users prefer this action because it is easier to predict the application of horizontal and vertical sketch constraints. 

 

Some users do not like the amount of view rotation and prefer to set the Look At Behavior to "Preform Minimum Rotation".

 

 

This setting will only rotate the view enough to align the sketch plane normal to the view and align the sketch axis with the view.  This minimum rotation may or may not align the dark horizontal axis to a true horizontal position.  Watch the video below and note the rotation is much less but that the dark horizontal axis ends up in a vertical orientation.

 





 

With this setting the user must pay attention to the axis orientation to make sure they use the correct sketch constraint when applying horizontal and vertical constraints.  If the user has configured Inventor not to show sketch axis, it is recommended that the Look At Behavior be set to "Align with Local Coordinate System" since it would be difficult to detect if the horizontal axis of the sketch actually ends up in a vertical position.

Continuing My Blog - Configuring a Custom Content Center

I created this blog about 4 years ago with the hope of using it to help others with their use of the Autodesk mechanical applications.  My company, Imaginit Technologies, soon after invited me to contribute to their Manufacturing Blog so I put my personal blog on hold.  I have recently retired and now it is time to begin to post articles on my site again.  I hope you will enjoy and benefit from these and I welcome any feedback you may have.

I thought my first new post would outline the steps to customize an Inventor Content Center library.  I am assuming in this article that you have already created a Custom Content Center (CCC) library. 



The Content Center Editor (CCE) can be found in two locations in Inventor.  From the Home page, the CCE can be found under the Tools tab on the Content Center panel.



With a file open, the same command can be accessed from the Manage, Content Center panel.  This makes it easy to work with CCC libraries during the editing process.

I am copying the Inventor DIN socket head cap screw (SHCS) to my library to be modified.  My main reason for this is the original library is too extensive and the naming scheme does not suit my need.

My first step is to remove the link for my copied CCC to the original.  Right click on the family and select "Suppress Link" on the context menu.

 

 

Next I will revise the Family Properties to better identify my CCC.    Again right click on the family and select "Family Properties".





In the Family Properties I changed the following fields.  Click OK when finished.

1. Family Name - This is the name shown in the CCE as the family name.
2. Family Description - This will be the name added to the iProperty "Description " field.
3. Standard Organization and Manufacturer - The name should be changed to allow easy Content Center indexing.
4. Family Folder Name - This is the name of the folder created in the Content Center folder that will contain the developed CCC components.

 



The copied CCC contains 855 SHCS entries, from M1.4 to M100 diameter, far more than I need.  I will select multiple lines and delete those sizes I do not need.  When selecting, use the RowStatus column.

One of the main reasons to create my CCC is to change the Part Number, File Name and the Inventor Browser name.  My standards do not follow the naming formats used by Autodesk.  For example the part number in the original table for an M10 x 1 x 30 LG SHCS is "DIN 912 - M10 x 1 x 30"  I will start with the "File Name" and edit the expression.  Right click on the "File Name" column blank area and select "Column Properties".



In the Custom Properties dialog box, notice the "Expression Column" format.  This expression is used to configure the information displayed for each row in the column. 

Below I have modified the expression to conform to my SHCS file name standard.  If you are unsure of the results of your expression, select "OK" and the column will update allowing you to see if your expression is correct.

I would also like this naming expression to be used as the Inventor Browser callout when the screw is placed in an assembly.  Select the "Map to Inventor Property" drop down and select "Member. Display Name".  Note that you can send the property to most of the standard Inventor iProperties as well as custom ones.  Only one mapping is allowed per column so it you need the same information mapped to another iProperty, just create a new column in the family table.



Before I leave the dialog box, I will highlight and copy the expression line.  I would like to use the same expression for the "Part Number" column.  Remember the Part Number is used by the Parts List in the drawing.  After copying the expression I select "OK" to close the dialog box and then open the "Column Properties" for the "Part Number" column.  the "Expression" checkbox must be checked to allow the pasting of the expression in the configuration field.  Select "OK" to finish.

 

 

The last step is to publish your changes.  You will notice all the fields that were modified have a yellow background and all the rows that were modified have yellow lighting bolts on them.  Select "OK" to publish and close the editor or "Apply" to publish and remain in the editor to continue working.

 

I want to validate my changes by creating and applying a CC filter to show my CCC and place a SHCS in the assembly.  Below you will see the results of my changes.