Autodesk Inventor

2D Draughting to 3D Models

HughLeave a comment

2D Draughting to 3D Conversion

2d to 3dTechnical drawings, detailing the specifics of your design can be critical for the communication both internally and externally. We can transform your 2D CAD or fully dimensioned legacy paper drawings to 3D Models using our experienced engineers to ensure drawings are 100% accurate and adhere to the most relevant standards and protocols.

3D Cad models will be fully inclusive of manufacturing tolerances as specified. New 2D drawings will be derived from the 3D model, dimensioned and denoted as original.

Attributes and BIM IFC data can be incorporated according to your engineering and company standards for Structural, Mechanical, Building Services and Equipment projects.

We normally use the Autodesk Inventor but are equally capable with all the Autocad based products from which we can provide native format model files or various other formats to suit your requirements, including DWG, IFC, STEP and STL.

We can provide CAD modelling services for your restoration project, adhering to all appropriate standards and design specifications.exit

NAA P-51D Mustang: Carb Air Scoop

HughLeave a comment

NAA P-51D Mustang: Carb Air Scoop

In an earlier post I discussed in some detail the progression of model development for the Carburetor Air Scoop (Lower Cowling) inlet and I mentioned that the final Air Scoop would be uploaded upon completion. Earlier Post : Air Scoop Prelim work:

It has actually been completed for awhile; I just forgot to upload it!

So here it is and if anyone has attempted to model a complex surface of this type you will understand how difficult this can be. Needless to say the Freeform T-Splines were invaluable in obtaining the correct surface.

The surface model is attached to over 300 ordinate points with numerous contour and fairing curves generated in preparation for the final surface modelling.

The data was first prepared in a spreadsheet; listing all ordinate points in mm and inch dimensions from which I extrapolated the 3D coordinates for each point; essentially creating a point cloud.

The ordinates were imported into Autocad, analysed and then the points grouped accordingly to define the contours and fairing lines.

This was then imported into Inventor and the surface painstakingly built up in each separate square grid attaching all the ordinate points. There was no easy way of doing this; I know I tried!

I am delighted to have finally completed this particular model having consumed many hours trying various methods to get it just right.

NAA P-51D Mustang: Project Cad Technote; Smart Parts Vb

HughLeave a comment

NAA P-51D Mustang: Project Cad Technote; Smart Parts Vb

I was looking at options for routing the cables in the tailwheel assembly. There is potential for a lot of ancillary routing for pipes and cables yet to be done in this assembly so I have deliberately shied away from the adaptive parts (which I am not keen on) and the typical pipe and cable routing functions.

Also the cables are comprised of end terminals and many are sleeved for part of their length, which would mean having to route several times if I was to do this using the routing functions.

What I really wanted to do is have a sub assembly that contains the cable with all its bits in one sub assembly file but using the coordinates from the assembly to ensure correctness.

Extracting point coordinates from an Inventor assembly is not that straightforward requiring as in this case a vb solution, but first I had to define the key points.

2015-07-23_02-51-10      2015-07-23_02-44-30      2015-07-23_02-46-01

I use the term “smart parts” and what this entails is for the parts or sub assemblies to contain additional geometry that will assist with other modelling activities like cable routing.

The image on the left shows the cables in this area with 2 key points 1&2 highlighted that are replicated in the 2 archive images. They define the straight section of the cable sleeve that is below and above the cable clips; the locations of which I have incorporated as points in the component sub assembly (last image). This sub assembly does not sit vertically in the assembly, the final position and orientation being determined by other factors which influences the final routing of the cable sleeve.

I have done something similar with the connection at the other end towards the left of the first image. At this stage I now have 4 points that determine the extent of the cable sleeve.

2015-07-23_03-13-17The next step was to go to the main assembly and extract the X,Y,Z coordinates of the four points from the fitted components.

I first select these and run a visual basic routine to extract the coordinates of each point and create a csv file which I import into excel which in turn is imported into a separate Cad part file.

It was then simply a case of running a spline through all four points and sweeping the sleeve profile.

The great thing about this is that the coordinates are relative to the origin of the main assembly so when I import the cable sleeve into the assembly I only have to constrain to the origin planes and it fits perfectly.

2015-07-23_03-23-16The cable itself will be done later in a similar manner which would be added to the sleeve part file as a multi part item or sub assembly using the sleeve centre line as part of the routing.

So no adaptivity, no complex pipe or cable routing just simple association through coordinate translations. The parameters of the sub assembly can be linked back to a spreadsheet so if the route changes I just re-extract the point coordinates and update the spreadsheet, which in turn will update the model.

To me this is a very tidy solution and maintains the integrity of the modelling hierarchy in accordance with the NAA register.

Using additional content in part files to facilitate other activities is very useful for examples like this and in fact any part that is associated with piping or cabling systems, particularly where you have cable clips or supports that need to be considered.

I should note that the extent of the cable sleeve is not exactly as shown in the first image due to the termination part not yet being modeled so I used something that was close at hand to demonstrate this principal.

If you would like a copy of the VB routine then please drop me an email and I will send it onto you.

NAA P-51D Mustang: Project Cad Technote Multi Body Parts

HughLeave a comment

NAA P-51D Mustang: Project Cad Technote Multi Body Parts

The process of developing these drawings into accurate 3d models relies on maintaining the hierarchy according to the original NAA drawings, even if sometimes it gets a tad confusing when dealing with what constitutes a “sub-assembly” as I mentioned before.

The sub-assemblies I described as “Part Assemblies” as the assembly unusually comprises a fully detailed part inclusive of additional items like bearing, spacers etc.

I have reviewed my approach to how I deal with this and thought it may be prudent to write a quick note on this technique.

I am utilising the multi-part feature within Inventor for this, which allows you to model separate solid parts within a single part file and then create an assembly that comprises some or all of these solids.

2015-07-07_12-57-05

This is a scrap view from the NAA drawing showing an assembly that has 2 configurations based on varying paired angles with spacers and rivets as shown.

Each of these items has a suffix added to the part number i.e -1, -2, -3 etc.

These images give you some idea of how I have modeled this, with the first image showing the configuration of items 2 & 3 and the second showing the configuration of item 2 & 4; all in one cad part file.

2015-07-07_12-41-28 2015-07-07_12-41-49

The beauty of working with multi body parts is that you only need one set of sketches that can be shared between all 3 parts.

2015-07-07_12-42-16

The sketches are dimensioned exactly as the original drawing…I mention this because I would not normally dimension from the edge of an angle section (cut edge); its not really good practice!

The image on the left shows the feature tree within Inventor; listing the 3 solids with appropriate suffixes.

The part file name (at the top) comprises the NAA drawing number with a suffix noting the archive reference.

All I have to do now is create an assembly for each of the configurations and add the relevant spacers and rivets. This is done very quickly using the “Create component” feature. The assembly number will comprise the NAA drawing number suffixed with either a -1 or a -5 respectively.

2015-07-07_13-50-22Only assemblies created from a multi-body part will be suffixed with a numerical character, otherwise they will simply be suffixed with SA.

Using this technique we maintain the integrity of the NAA numbering system with an hierarchy that suits the CAD strategy.

In a previous post I discussed “as-fitted” parts; like bushes; that might be press fitted and and reamed thus dimensionally different from the manufactured part, so these will still be modelled within the part file to “as-fitted” state and not brought in as a component of the sub assembly.

NAA P-51D Mustang: Tail Wheel Assembly Update

HughLeave a comment

NAA P-51D Mustang: Tail Wheel Assembly Update

I rather enjoy building these Cad models and the challenges they represent, however I still have a lot of work to do with organising the archive materials and the document register; which I briefly mentioned in previous posts.

I have decided to adopt a BIM methodology for the organisation and restructuring of the archive datasets and to look at the options for managing the content and format of the tagged properties within the 3D CAd models.

This all needs to be done, so I will take a break from modelling the parts for a while to concentrate on developing the above. So on this last day I decided to tackle some of the smaller parts for the eventual Tail Wheel assembly for the P-51; which surprisingly were interesting parts to build.

2015-06-26_21-14-15 2015-06-27_00-36-57

#73-34189: Bell Crank: Steering Pulley               #97-34172:Retainer: spindle lockpin

2015-06-27_18-08-13 2015-06-27_00-39-04

# 97-34191: Bracket Torque Tube Pulley      #73-34515: Bell Crank – Retract position lock

There are also a lot of parts that don’t have drawings in this archive; mainly aviation standard parts for bolts, washers, seals and bushes for which I need to knuckle down and source the dimensional information so that I can build the requisite part model libraries.

There is still a lot to consider as I move forward with this project!

NAA P-51D Mustang: Tail Wheel Down Position Support

Hugh3 Comments

NAA P-51D Mustang: Tail Wheel Down Position Support; Derived Parts (Inv)

I mentioned in an earlier post that we don’t have many of the forgings/castings for this aircraft but the few that we do have are not stated as such in their description and thus occasionally overlooked.

In this case the forging/casting was noted in the NAA machining drawing; which I do have.  This gives me an opportunity to explain one of the strengths of the Autodesk Inventor product, namely derived parts!

Derived parts are a powerful but easy-to-use tool that comes in two basic flavors: you can derive a part from another one, or you can derive a part from an assembly. Using derived parts, you can easily create machining models and drawings from an as-cast model, and you can create a mold from the same model.

2015-06-25_23-39-08 2015-06-25_23-38-08

These images show the casting model I created from the original NAA drawing #73-34162 for the Tail Wheel Down Position Support.

This model took me quite a while to do due to the creation of all the fillets which got a bit crazy sometimes and I ended having to redo them several times to get them the way I wanted.

2015-06-25_23-39-27 2015-06-25_23-37-48

The machining model is a separate Cad part file created from NAA drawing #73-34161 which has the casting body and sketches derived from the first Cad model above. I can now go about working on the derived model; creating the machined elements and holes; without affecting the original model file above as shown.

The great thing about working this way is that should the original casting model change then this will be propagated to any other cad part files to which this item is derived but conversely any changes in these Cad part files are not reflected in the casting model.

I still have a few minor details to finish this model but thought it may be prudent to touch on the derived part capabilities of the Inventor product.

Another use for derived components is when you only have Inventor LT (Lite version) which is a parts only product and unlike its big brother does not handle assemblies. Using the derived feature it is possible to create a proxy assembly for checking the alignment of parts as shown below.

This is the armor plating for the Mustang P-51 Firewall; with the top section modeled separately from the bottom section. In this example, I have derived the top part into the lower part file as a surface model to assess the alignment and curvature continuity.

Autocad Inventor: Splines

HughLeave a comment

Spline Technote:

Splines are an absolute necessity when developing the finished profiles from the ordinate points; which occasionally throws up some unexpected results.  Invariably at some point we need to manage the curvature of the splines in order to achieve the desired result.

2015-06-09_10-15-47

The image shown here is a screenshot from the NAA P-51 fuselage station profiles, which shows clearly the ideal curvature for each station.

This image can be overlayed in CAD to serve as an aid to achieve the correct spline curvature.

Actually manipulating the curvature of a spline needs to be done in a manner that achieves symmetrical results on both sides of the fuselage station profile.

I was working on the tail-end profiles, which were giving me grief as the ordinates points were not sufficient to achieve anything close to the curvature I needed on the lower section.

2015-06-09_13-26-35

In Inventor we have constraints for symmetry, which are normally applied when working on a sketch to ensure that changes on one side of a model are reflected exactly in the other.

Using this same technique I activated the spline curvature handles (A&B) on each of the  points I wanted to be symmetrical (about center at C) and applied the constraint accordingly to the handles (red).

2015-06-09_17-29-44Now when I adjust one side of the curve the other side automatically reflects the changes.

I should note that the majority of curves generated from the ordinate points are usually very good; requiring very small if any adjustments; so its quite practical to spend some time in the areas where they are not so good.

At some stage the profiles will be lofted as a surface which would then be analysed to verify curvature and alignments.