Autodesk Inventor for Woodworkers: Gottshall Block Part Modelling Exercise.
Some of those old Woodworking exercises you did way back when you were just starting out might be just what you need to help you learn Autodesk Inventor!
I have been really enjoying this series of posts on One Old Exercise for Growing Skills from Robert W. Lang over at Popular Woodworking Magazine.
In his series, Robert takes a drawing from Franklin Gottshall’s Making Antique Furniture Reproductions (suggested by Mike Wenzloff) and takes us through the various steps of the exercise from marking out to the finished block.
Of course I couldn’t help but whip up my own version of the Gottshall block!
How to create a 3D model of a Gotshall Block with Autodesk Inventor
Here’s Franklin Gottshall’s original drawing above…
And here’s my version below…
(you’ll notice I have dimensioned it with dual units, and used modern English terms).
There are many different ways that this item could be modelled inside Inventor. Just to keep it interesting I’ve tried to use some of the less obvious methods.
Adding Parameters
The first Job is to add some Parameters. Notice that even though my template file is in Millimetres, I have added all the values in Inches.
Tip: Type ‘in’ or ‘inch’ after the value to let Inventor know what you want.
Inventor will convert the fractional inches into decimal inches and will even add up values with fractions that have different denominators (That saved me a lot of headaches, I can tell you).
Here’s my master sketch. I’ve tried to use the minimum amount of geometry – so it looks a little cryptic.
Adding Workplanes
Next job is to create some Workplanes. I prefer to use work planes rather than working off other features. That way, if I need to edit a feature, I stand less chance of messing up any other features that were depending on it.
I’ve created one more sketch here for the concave cut. Note that I have made one end of the loop into centre line geometry.
Creating a Base Feature
Rather than extrude the base feature I thought I’d show this technique. First I use the ‘Surface’ option in the extrude command to create a work feature…
Then I thicken the work feature to create the solid. The whole solid is based on one single line of geometry. No loops = no loops to fail!
Creating Cut Features
I’ve used The various flavours of the Extrude tool to create the Cuts features.
In this case I’ve used the ‘From to’ option– Using the work planes I created earlier.
I have formed this cut using the ‘Distance’ option, which is set to the ‘Thickness’ parameter value.
Pow! a Cut through all!
Finally a ‘From To’ cut, using the faces of the original block itself (Usually a bad idea…)
The fillet with the ‘Fillet’ tool…
…And the Chamfer with the ‘Chamfer’ tool (No surprises there!)
I created the concave cut with the ‘Revolve’ tool – which is what I needed that closed loop with the center line geometry for.
For my final trick, I created the rebate on the end of the block with the ‘Lip’ tool from the new plastic parts tool set.
In conclusion
You probably won’t learn as much from my tutorial as you would from Roberts! I hope that I’ve thrown in a few unusual suggestions, why not leave a comment and tell me how you would do it.
You can download the Part file and a PDF of the drawing here:
[Download not found]If you are so exited about this article that you decide to download the Inventor file – Please leave a comment!
If you would like to find out how to turn your parts into assemblies – read Assembly Techniques for Wood workers.
Why did you say:
From To’ cut, using the faces of the original block itself (Usually a bad idea…)?
Thanks for the tutorial – a different approach is always welcome
Hi Ben,
I wrote this post some time ago – so I can’t quite remember my train of thought here…
In general, I recommend creating the fewest number of relationships possible, so a cut extrude with distance set to ‘All’, is safer than a ‘From to’ cut…
Does that make sense?
Paul
Otra perspectiva interesante de cómo hacer las cosas aun cuando estas sean sencillas, muchas gracias por compartir el conocimiento
Hi Hugo,
From Google translate:
‘Another interesting perspective of how to do things even though these are simple, thank you very much for sharing knowledge’
Thank you Hugo!
Paul
I was able to place dimensions, not the text ‘REBATE’, ‘HOUSING’, etc. Placing text on an .idw does not give oblique text. I produced desired results by creating a dimension stlye without extension lines, arrows forced outside (eliminated the dimension line) and no arrowheads.
Thanks for the response. Nice website.
Ahh! Good question.
You know what – I forgot how I did this myself. So I went back and took a look… and you know what? Apparently I cheated and did the text in AutoCAD.
Oh – the shame!
(The dimensions where all done in Inventor though!)
Thanks for the tutorial. I’ve been using Inventor for 4 years and using the surface extrusion and thicken to create a solid body was new to me.
I have never done annotation on an isometric before and was trying to recreate your detailed isometric. How did you create your oblique text?
Hi M. Scott,
You are using Inventor right? (Just checking!).
I just clicked on the points/lines that I wanted to Dim and Inventor did the rest.
Once you have the geometry picked, before you click to place the dimension, hit the space bar to toggle the dimension plane.
There is also a setting for default dimension plane – which is usually set to ‘model’, but could trip you up if it has been set to ‘paper’. To get to this, right click on the view boundary and look for the dimension plane option.
I hope that this helps – let me know how you get on!
Paul