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Using Autodesk Inventor to create a notched wood construction (Jeweler's Bench Tool Holder)

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Picture of Using Autodesk Inventor to create a notched wood construction (Jeweler's Bench Tool Holder)
As I spend a lot of my creating time on making jewelry, my jeweler's bench gets covered in tools so I needed more storage space for my tools. So I designed this tool holder in Inventor and as doing it I thought it would be good to share some of the techniques I used in the design process. So here it is.

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Step 1: Initial Design

Picture of Initial Design
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The first step was to design the tool holder in Inventor. Each piece will be cut from 1/4 inch piece of wood with a laser cutter. For this we need to design each piece as a separate Inventor part.

Step 2: Assemble the Pieces

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After the pieces are modeled they need to be assembled to help define where to cut the notches. The image provided shows how each piece is overlapped during the assembly.

Step 3: Add a Parameter for Kerf

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As I mentioned we will be cutting the pieces out using a laser cutter so we need to keep the Kerf in mind when adding the notches. For more information on Kerf see this Instructable. For each piece we will add a parameter to adjust the tab size on the fly. To add the parameter select the "Manage" Tab. Once the Parameter dialog box is up add a parameter named Kerf and set the value to the Kerf of the laser cutter being used to cut the pieces.

Step 4: Add Notches

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When adding the notches draw the notches with construction lines first. After adding the construction geometry outline the construction geometry with regular geometry and add a dimension between the construction geometry and regular geometry make the dimension value the parameter Kerf. This will allow the adjustment of the Kerf by simply changing the parameter. 

Step 5: Layout the Pieces for Cutting

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Using an Inventor drawing place a flat view of each piece needed to be cut on the drawing sheet.
0rel8 months ago

Great, exactly what I want to learn more about right now - thanks for sharing!

violator831 year ago
Ok, installed inventor, I made all parts I need for my project by simple forms and extrusion but now that I try to assemble them to this stage I'm really getting mad. How have I to do to join parts to obtain a thing like this.
togo19191 year ago
Tom-
I'm trying to import a box design to Inventor, then modify the tab length for all tabs, based on the thickness of the material. (plastic, plywood, mdf, etc) I'm using Boxmaker to create a pdf for the box design.

I can get the pdf to dwg okay and import to Inventor just fine.
Any guidance on how to set up constraints (or another method) so I can modify my drawings easily/quickly based on tab size? (shorter tabs for thinner material and longer tabs for thicker material)
Thanks,
TG
TomCloss (author)  togo19191 year ago
The short answer is, to use a linked spreadsheet. I have a feeling you might need more than one variable. I could have done this for this particular project but seeing as I was only using one variable, I didn't. From the manage tab in inventor you can select parameters. Use the "Link" button in the parameter dialog box to link each part to the same spread sheet.

A couple of thoughts I have is the number of notches may need to change. This means you might have to redraw the sketch and apply the notches using an array. Also be careful when adding assembly constraints. You don't want to add a constraint to a notch or feature that might not be there if you change the thickness. Just my two cents.
Thanks for the guidance. I made big advances this weekend on the design - using a total of 5 variables - material thickness, box inside width, box inside height, box inside depth, tab width.

I'm definitely feeling better about constraints - I'm sure I'll be learning plenty more about them...
Nice technique and the holder looks great :) You should enter this into the Holiday Gifts Contest!
TomCloss (author)  Penolopy Bulnick1 year ago
Thanks for the encouragement. I don't think I am disqualified from entering contests since I work for Autodesk Consulting by day.
togo19191 year ago
I'm devoting lots of time this month to getting into the 3D realm with Inventor. Thank you for the timely posting!
wilwrk4tls1 year ago
I have a couple of ideas to maybe help simplify the parameter changing:
1) create an empty skeleton file with the parameter Kerf in it, and in all of your part files create a linked parameter, linking to the empty skeleton file's Kerf parameter. Then you can change the Kerf in the skeleton file and it will update in all the part files.

2) Create all the different parts in one part file, with extrusions set to create a new solid when you need a new part. You can use one parameter for Kerf inside that part file, even accross new solids. Once all the parts are modeled, use "Make Components" and export the solids into a new assembly. They will all update at once when you make changes in the base part.

That's somewhat simplified as far as going through the process, but I have found it very helpful (method 2) when constructing assemblies that require a lot of common fastening locations, etc. because Inventor usually crashes when projecting geometry across parts in an assembly. It allows you to use all of the parameters in one part file for an entire assembly of parts since they are all created from one part originally.
TomCloss (author)  wilwrk4tls1 year ago
These are great suggestions. I've used similar techniques in larger assemblies. Thanks for the suggestions.
Wow, that came out really nicely! Would you be willing to share your laser cutter files in this instructable? Thanks!
TomCloss (author)  audreyobscura1 year ago
Sure, here is the inventor files so someone can adjust the Kerf as needed. If someone wants a Corel Draw version or a DXF please let me know and I'll create them and post them as well