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Selecting Continuous Segments in Inventor 2008

When selecting continuous segments in Inventor 2008, if you leave the Merge option unchecked, the selected geometry will create individual frame members; if you leave the Merge option checked, the selected geometry will create continuous, bent frame members.

Inventor: Centralized Content Repository

For the workgroup or larger installation, the Content Centre can be deployed as a centralized content repository. You can customize the content data (part number, descriptions, and more) based on company preferences so designers work with the same approved data. (Inventor R11 SP2+)

Quickly Use AutoCAD Sketches!

You know when you want to copy a complex profile quickly from AutoCAD and you paste it into a part sketch the entities are not constrained and require a tedious and timely effort to fully constrain! Well follow these steps to solve this issue in a jiffy.

1. Start a new sketch in a part file
2. Make sure ALL projected sketch geometry is deleted including the popular centre point!
3. Copy (Import or Paste) your sketch into the blank ipt sketch
4. Now choose the Auto Dimension Tool and select Apply (you may need to check the Dims and Const options)

Poof the sketched profile is now completely dimensioned and constrained within it's self! ...and now you can project geometry and apply constraints to lock its positional requirements!

Note: This is NOT the best way to model but a quick solution in some cases!

How to open Assemblies with desired LOD automatically

Currently you have to use the Options dialog in File Open to set the desired LOD that you wish to open your assembly in. However if you make a copy of your Inventor shortcut and in the target properties paste the file location with the desired LOD in the less than greater than square brackets after the file name (the same as in the Recently used file list displays in Inventor) They can't be typed here as they won't show in HTML.

See the link below for a screen capture of the Inventor shortcut target (copy and paste into your browser)

http://discussion.autodesk.com/adskcsp/servlet/JiveServlet/download/78-540962-5478003-138993/Untitled.jpg

Using Face Splits to Control Welds

Problem: Getting Properly Spaced Fillet Welds in Inventor Often it is impossible to get properly space and locate fillet welds in Inventor, due to the model geometry properties. In this example, the round part will "chain" the weld around the face. Individual partial face welds may not be placed properly in relation to the base part.

One solution to this problem is to make a face split on the base part to allow control of the exposed base face inside the face split.

In a sketch: when starting a line

In a sketch: when starting a line from the edge of a circle, select the start point on the circle then hold down the shift key as you pull the line away. If you were close to tangent it will hold the tangent constraint as you pull the line around the circle and place that constraint when you pick the end point of the line. If you were closer to radial, it will hold the line radial to the circle as you drag it around and placed two coincident constraints when you pick the end point (one on the circle edge to the beginning line point and one from the circle centre to the line).

Horizontal or Vertical – Autodesk Inventor 2D Sketch constraints

Have you ever started a sketch on a part and wondered, “do I need the horizontal or vertical constraint?” As you apply new sketches to parts and use the “Look at” command, your part will rotate relative to that plane. There will be times when you will add a geometric constraint and it will be wrong. For example, say you want to add a horizontal and you apply that to your sketch and the end result is not what you expected. The constraint should have been the vertical constraint not the HORIZONAL constraint.

If you are having this issue, here is the tip for you. The secret lies within your sketch axes. When you start a new sketch, look to your gird lines and the boldest grid line on your graphics screen is the X axes or in laymen’s terms the horizon. By following this you will never have to question yourself again, horizontal or vertical.

Equally "Divide" using a Reference Dims

Environment: Part Sketch

Examples:

1. Equally Divide centre points along a linear path
2. Create Symmetrical relationships with only centre points

when placing Point, Hole Centre (PHC) along a linear path you can quickly divide the spacing equally by linking the spacing of each PHC to a reference dimensions. For example if you have a sheet metal panel and the mounting holes are placed along one edge with each corner mounting hole offset from the adjacent sides by a different value due to design, you then can divide the other mounting holes equally between the given space between those corner holes.

Here's How:

1. You would first fully constrain the two PHC by their respective distances (be sure they are linear aligned)
2. Then place a few (2 or 3) PHC linear aligned between them
3. Now place a dimension from one corner PHC to the next relative PHC
4. Continue placing additional dimensions until the last one is dimensioned to the opposite corner PHC to which you started
5. The last dimension you placed will default as a Reference, that's ok!
6. To equally divide the spacing of these PHC you will need to edit the values of the "non" reference dimensions to equal the reference dimension

Assembly Tools (R10, R11& R12)

There are some useful Assembly tools to be found in the SDK folder:C:\Program Files\Autodesk\Inventor 2008\SDK\Tools\Users\AssemblyTools

Rename Browser Nodes: Brings up a dialog to allow fast renaming of component occurrences in the assembly browser. The: available choices are "Filename" (display file name of the document from which the component occurrence: (has been inserted), "Part number" (the part number file property of the document), or "Default" (the: default browser name that Inventor provides for component occurrences).

Add Part: Similar to Inventor's default "Create Component" command, however it bypasses the Type selector, : and goes to a "Parts" directory as the new path, if it is seen in the project folder. Further, it : does not prompt for a sketch.

Add Assembly: Same as above, only for assemblies, and assumes "Assemblies" as a directory.

Save and Replace Component: Takes the selected component, runs a "Save As" command (with name prompt), and replaces the selected: component with the newly saved copy of the component.

Ground and Root Component: Takes the selected component and moves it to the origin of the parent, and grounds it.

Alpha Sort Components: Sorts the names of the components that are displayed in the model browser in alphabetical order.

Component Derive: This command streamlines the implementation of built-in "Derived Component" command in the part : environment. After user selects a base component (part or assembly), this command generates the : derived part or assembly using the default options as offered by the built-in command. The only: exception is in representations: this command will imply base component's active design view: positional, and level of detail representations to be used in derivation.

Place at Component Origin: Similarly to "Place Component" in the assembly environment, this command adds a component : occurrence to assembly; however, the new occurrence is placed at the origin of selected existing : component occurrence, by mating the corresponding origin work features between two components.

Un-share sketch in Inventor 11

If you have ever wanted to unshare a sketch, you now can in Inventor 11. If you share a sketch and realize it is only used in one feature you can RMB on the sketch and select Unshare.

Create multi-pitched helical sweep

Inventor R11 now includes the ability to easily create a multi-pitched helical sweep. Create an extruded cylinder as a surface e.g. 10mm dia x 100mm high Create a sketch tangent to the cylinder face. On the sketch create a line that is collinear with the end of the cylinder. The sketch then needs to include all the pitches, the horizontal length of the line should be the circumference of the cylinder (31.42mm) and the vertical pitch of the line should be the helical pitch. Exit the sketch once complete. Create a new 3D Sketch and select Project Curve to Surface. Choose the cylinder face as the face and then select the individual parts of the sketch you wish to project as the Curve. Make sure you select Wrap to Face (third icon along) hit apply..... You're 2D sketch will now be wrapped as helix around the cylindrical surface. Use boundary patch to close the cylinder, stitch it together and you now have a solid that has a 3D multi-pitch helical sweep wrapped around it. Use the updated tools in Sweep to cut your path.

R11 - Curvy Stuff - 1

New in Inventor R11 there is a whole stockpile of wonderful tools for shape description. Just today I learned about the new loft to a point option. Now when lofting you can choose a single point for your shape to end on. At first pass sounds kind of weird, wait till you see the preview:). Then on the "conditions" tab you can adjust between SHARP, TANGENT, and TANGENT TO PLANE. Have fun.

Creating multiple views in a model

Sometimes being able to view your model or assembly from a few different camera angles can help while making design choices. Using the pull down menu Window>>>New Window, will create a new window of the active document that you can resize as needed or tile to see two views at one time.

Use Endpoints of Lines for Holes 2

In addition to the original tip you can also highlight geometry while in a sketch and then select the 'Hole Centre' tool (little crosshair icon) on the standard toolbar to convert naturally occurring points to Hole Centres. When you start the 'Hole' tool those points will automatically be selected for hole placement.

Example: To place a rectangular hole pattern on a face try sketching a rectangle, selecting the geometry (using a window) and switch the 'Hole Centre' tool on. Then start the Hole command.

When projecting cross part geometry in an assembly file

When projecting cross part geometry in an assembly file, you can avoid the geometry, sketch, and part from becoming adaptive by holding the ctrl key down while selecting. This will project the geometry and place the "lock" constraint on it in the sketch.