Restoration Project: Corsair F4U-1

Restoration Project: Corsair F4U-1

This is great news; a good friend of mine has just acquired the wreckage remains of a Corsair F4u-1.


The long-term plan is to restore this Corsair to its original specification as a standing exhibit. It would be wonderful to restore to flying condition but the projected cost as it stands is quite overwhelming and to achieve flight status would probably double that.




We will be setting up a dedicated blog and website to record progress on this restoration. Part one of the project is to develop a master lines plan which will be used to design the jigs required to rebuild the fuselage and wings.

Any contributions to the project, regardless of how small will be greatly appreciated.

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Technote: Inventor LT BOM!

Technote: Inventor LT Bill of Material.

I normally use Inventor Professional but recently I decided to have a look at a common issue with Autodesk Inventor LT which is a part only product. Essentially the “lite” version of Inventor with limited functionality that excludes sheet metal, vba, ilogic, assembly mode and Bill of Material!. Technically the BOM capability is not a function of Inventor LT which I suspect is due to the fact it has no assembly environment but there is a workaround.

I should note that Inventor LT is a very capable modeling product which is ideal if you are mainly developing parts and if you do require an assembly environment to check the alignment of mating parts then you can use the derived function as explored in a previous post to assess this.

Whilst the product may be limited it does have a lot of functionality that can be exploited to overcome some of the limitations and the BOM is just one example of a situation that the forums, in general, described as something that cannot be done!

For this example we will continue with one of the parts from the previous article: the Bell P-39 Airacobra Centre Bulkhead fixing bracket.


What I wish to do is have this part fully dimensioned on a drawing that also contains a basic table of properties that may be useful to the chap responsible for buying the raw material. Okay, I accept that the following image is not fully dimensioned but my primary interest is the generation of the BOM.


Inventor LT like its bigger brother contains a lot of part data which is accessible via the iProperties and Parameters, which we will utilize by using the iPart feature.

Normally iParts are used where a single part may come in varying sizes or configurations that share the same basic features; for example bolts! In this case we are creating only one version of the part. By adopting the capabilities of iParts we will create a table of selected data within the part file that we will later use as a data source for our BOM.


I won’t go into the technicalities of creating an iPart, there are many online resources that go into this in detail. Generally speaking, when creating an iPart you have access to all available data including parameters, model hierarchy data, and iProperties as shown above and it is simply a case of selecting the data you want.

2017-07-31_15-52-34This creates a Table which appears in the model browser. It is usually a good idea to give parameters meaningful names as I have done here for the Length, Width and Height.

The Description values are from the iProperties whereas the Length value is from the parameters.

This table can be further edited within Inventor LT or externally as an excel spreadsheet.

In the drawing environment, you select the General table option, Select View and then Column Chooser, add required columns, select OK and insert the table into your drawing.


…and there we have it…a BOM in an Inventor LT part drawing.

Part Quantities:

I have not mentioned part quantities which of course would be a prerequisite for any purchasing decision. You can, of course, create a parameter in the model file for quantity and include that in the table, but if this part serves a number of different assemblies then the quantity will vary accordingly.

Given a typical scenario where you are the manufacturer of components working collaboratively with other companies on a project how do you track quantities when you are using LT and the other guys are using Inventor and building assemblies.? You could, of course, just phone them or email them but as production schedules are critical you need a way of immediate notification of quantity changes.

I faced a similar dilemma when I developed a modular solution for a power distribution company for design of sub stations. This resulted in vastly reducing the design time by over 60% which meant the procurement chaps had to up their game to keep on top of things.

Modular Approach to Sub-Station Design

The solution gave access to all project material BOMs without needing to bother engineers to create structured BOM extractions.

Briefly what we had was a top level assembly BOM which was interrogated by a custom database application to read the Part Name column and then search a folder of extracted cad model BOMs with the matching name and multiplying the quantity column in the part BOM with that of the assembly.


For example, the database would open the top level database above, read the columns Name & Descr (to be sure we were only looking for modules) and then import the corresponding data files with those names into the database. In this case, we only have 1 quantity per part, but that could be anything and the associated part file would be multiplied accordingly.

This is a very basic overview of what was done and beyond the scope of this blog to describe in detail. We have already demonstrated how to create and extract tables in LT and the main point here is though you may only have Inventor LT there are many options for creating data-sets in tables that can be shared and used productively in a collaborative environment.

Incidentally, the database I created was another of those instances where something could not be done!

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Technote: Inventor Sketch Datum

Technote: Inventor Sketch Datum Point.

This is one of those instances where you do something on a regular basis and don’t really appreciate the significance of the process. What I am referring to is when you create a sketch Plane using the option “Parallel to Plane Through Point”.


It transpires that this selected point becomes the datum for the particular sketch created on this plane. For this example, for a P-39 wing rib, we have selected a point for the Plane location along the wing leading edge as shown.

P39 wing1

The Bell P-39 and similarly for the P-51 Mustang the wing ordinates are set out from the leading edge of the wing so it makes sense that the rib sketch is setup with a suitable datum point. You can tell the location of the temporary datum in the sketch applied to this plane by the position of the main axis.

This is the really interesting part, when you now import a set of points from the Ordinate spreadsheets it will recognize this sketch datum and import the points relative to this point irrespective of the model origin.



This is very useful particularly for these aircraft projects as we tend to use a lot of ordinate data for the outline geometry.

Another Quick Tip:

To automatically apply a tangent constraint to a sketch line just select and drag the line from an existing line and the tangent constraint will be applied.


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Technote: P-39 Inventor Facedraft

Technote: Bell P-39, Inventor FaceDraft

Draft angles is actually a common requirement when working with aircraft components, particularly forgings, and it is surprising that I haven’t written an article on this before now.

Facedraft in Inventor is a feature that allows adjusting the face or faces of an object to a specified angle. A more detailed overview is described in this Autodesk article Face Draft feature

Occasionally the implementation is not quite so straightforward as noted therein and some outside the box thinking is necessary. Thus was the case when I was building the forging component for the P-39 Landing Gear Nosewheel Scissor.

To build this component I created 2 separate solid bodies, one for the cylinder item and one for the fork. The fork is split about the X,Y plane with only the outline of the top half being modeled to facilitate the initial face draft.


For the first option, I selected the X,Y plane and then for the Faces I selected the automatic face chain option and placed the cursor close to the top edge as shown. If you required the face angle to originate from the bottom edge then you would select the faces close to this edge.

I then trimmed out the inside profile of the fork and applied a face draft as above.


Now it was only a matter of mirroring the fork solid to complete this portion. Notice the solids are still separate items which will be combined as one after inclusion of the central web component.


There is an option for the Facedraft feature to Draft using a parting line, either a 2d or 3d sketch. The draft is normally applied above and below this parting line. In most circumstances, the Parting Line option works well but occasionally the model may be too complex to achieve the desired result thus the solution described here provides an alternative approach.

Forgings or castings commonly have a draft angle on all faces which is normally 7 degrees and occasionally 5 degrees. The Face Draft feature is ideal for applying the drafts with an extensive range of options. The model of the forging would then be derived into a separate part file and then machined according to the finishing requirements similar to the process described here Derived Parts.



For more information on the Bell P-39 Airacobra project: Bell P-39: Project

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Technote: Inventor Export Sketches

Technote: Export Sketches

The Inventor product has an option to export part Sketches to either an Autocad DWG or DXF format directly from the model environment. This is very useful if you are needing to share development information with someone else who is working with a different CAD product.

It is simply a case of highlighting the sketch as shown in the example below and selecting the “Export Sketch as…” option.

Inventor export sketch

A dialogue box pops up asking for the file format DWG or DXF and location for saving. I would recommend the DWG for the format as this replicates the Splines more accurately.


In this example the left image is for the Mustang P-51 rear fuselage, showing the outer profile for the P-51 B/C and the inner profile is for the P-51D. The image on the right is the fuselage tail-end.

I plan on extracting all the fuselage curves that include P-51D data to DWG format as a reference until such time as I can add the point data to the already comprehensive set of ordinates available here.

Mustang P-51 B/C Ordinates


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Technote: Inventor Quick Tip

Technote: Inventor Quick Tip

Inventor taskbar

When working in Inventor you can access a list of Recent files by clicking the right mouse button on the Taskbar icon.

This also works for most programs with an icon on the Taskbar like Microsoft Excel, Notepad etc.

Posted in Aviation, Inventor, Technote | Leave a comment

Technote: Complex Surface Hole Location

Technote: Positioning Holes in Complex Surfaces

When detailing the skin panels for aircraft it can be quite daunting trying to locate a series of holes accurately at a specified distance from the edge of the panel. Typically fillets to wings and horizontal stabilizers and transition pieces to vertical stabilizers are all complex surfaces.

In this example, we need a series of holes located 17.5 mm from the top and bottom edges. As you can see the surface at the top and the flange angle at the base varies.

The location of the first hole, top and bottom, is aligned vertically so we first create a workplane to determine the horizontal position of the first hole. Ultimately we will use a 3d intersection curve for the centre line of the holes which must first be determined by sweeping a circle profile sketch along the edge as a surface with the radius set to the required edge distance. Using a circular profile for the sweep ensures that any intersection point on the surface will be at the specified edge distance.

This swept surface is then trimmed to the first work plane to define the start point of the 3d surface intersection curve as shown.

The resulting 3d spline represents the line of the hole centres at 17.5mm from any point along the edge of the fillet.

We then apply a point and an axis (perpendicular to the surface) at this point to determine the hole direction. I suspect because it is not a regular surface the hole feature will not allow me to select the surface for direction. Use “Extend Start” when creating hole.


To pattern the hole along the spline and be perpendicular to the surface create the array as shown below. Be sure to select the extended options for “Direction 1” and “Adjust”.


Do the same for the top array of holes, resulting in 2 sets of holes aligned with the surface at 17.5 mm from the edge.


This works for the vast majority of riveted panel connections where locally there is a degreee of flatness between the matching parts. In instances, where there is extreme curvature of the connecting faces the radius of the extruded circle would have to be adjusted accordingly.

Posted in Autodesk Inventor, Aviation, Fuselage Panels, Technote | Tagged , , , | Leave a comment