Assembly - compensate for hard anodize thickness?

[paulV9CCG]

We are designing a large measuring instrument assembly made of custom aluminum parts. All parts must fit with close tolerance to produce the required accuracy. The parts will be hard anodized, which adds approximately 0.002 inch thickness per side.

How should we take this thickness into account? Do we need to reduce each part by 0.002 inch and then use joints with offsets? This method does not scale well when dealing with many parts. Is there a better way?

[TrippyLighting]

You missed most of the important details.

Who is going to manufacture this device ?

Is the machining done in-house ?

Is the hard anodizing done in house ?

Is assembly done in House ?

If it is outsourced, have you talked to the supplier and what feedback have you received ?

The answers to this question all might drive the design.

They have in my almost 30 years of engineering!

[paulV9CCG]

We design, machine, and assemble. The anodizing is outsourced. We have spoken with the supplier and determined the build-up amount (0.002").

Since these are multiple parts that must fit tightly together, we need to machine them smaller by the anodizing build-up amount.

Our question is with respect to the Fusion 360 software: since we are designing for manufacturability, how do we handle this in the most efficient way and minimize mistakes?

Should we model in final net dimensions, so that the model represents the finished equipment correctly? Then, how do we compensate efficiently (and with no mistakes!) for the anodizing build-up when going to CAM and generating machining drawings?

Or, do we have to model incorrectly, with gaps between the parts, to accommodate the machining / anodizing process?

[n8bot]

How complex are the surfaces that require anodizing? Simple planar/cylindrical surfaces?

How many surfaces mate, and will be affected by the anodizing?

I imagine not EVERY dimension of your part is critical to 2 thou for fit, so I suggest you add the tolerance only to the areas that are critical. This can be done with a custom user parameter setting the tolerance once and re-using it anywhere that will be needed. You would definitely want to hard model the tolerance into the model. Any joints that you identify that will be affected can be modified parametrically by referencing the user parameter, to ensure they reflect the post-anodized function.

Are you familiar with the use of user parameters? They can be found by selecting the drop down in the Modify toolbar and choosing "Change Parameters." You can then define parameters and reference them by name in any dialog box. Although, be sure the units all match or you do not get full parametric functionality.

Alternatively, you could manage the tolerance in the CAM stage at some point, but I have little experience with that aspect of Fusion.

[TrippyLighting · Accepted solution]

Good feedback!

At the beginning of the design I would design everything to nominal / ideal dimension. This will capture the design intent better.

Just like it is an old engineering and CAD guideline not to apply fillets/chanfers at eh very end of the design stage, correcting part for anodizing allowance would be done at the end of the design and timeline in Fusion 360

Try to avoid linked comports as they will complicate this. What is your experience level in Fusion 360 ? Are you familiar with Fusion 360 R.U.L.E #1 ?

Remember that there is a timeline!

When the design is complete and everything is assembled a I would offset all surfaces or mating interfaces using a user parameter as @n8bot suggested.

I'd group these in the timeline and call the group Anodizing allowance, for example so it is clear what you are doing.

I can make a little screencast if that's not clear.

[paulV9CCG]

Thank you very much for your input.

To answer some questions:

@n8bot, the surfaces are simple planar / cylindrical (such as pockets, shafts, etc).

@TrippyLighting, thank you for R.U.L.E. #1. We have been using it.

Here is a very simplified example of my problem:

http://a360.co/2vRoEvK

Our finished product includes a large tooling plate with many subassemblies that must align correctly, some move on rails.

The model shown here is a simplified representation of one such subassembly. It shows three parts which must fit together with tight fit, meaning they can be assembled / disassembled by hand but with negligible clearance. If we add type 3 hard anodizing which builds up each surface (0.002"), these parts will not fit. So this represents our exact issue.

We like the idea of modeling to final dimensions and using a parameter to apply offset at the end, before going to CAM, as suggested here. But, being newbies to Fusion 360, we need a little help. 🙂

Once we create a parameter, how do we apply it so that the surfaces will move in the correct directions, without causing problems such as circular references, misalignment, and errors related to loss of geometry used in calculations. (Being new, we've run into those issues more than once.)

[n8bot · Accepted solution]

When using the offset faces command (by pressing Q and selecting the faces you want to apply the tolerance to), you want to remember to set the "Offset Type" drop down to "New Offset" so that a new feature will appear in your timeline. 

After you have defined the user parameter in the change parameters dialog, you can simply put the name of that parameter in the input box for the offset distance. If you need to reverse the direction of the offset, simply add a minus sign ( - ) in front of the name of the parameter, and it will reverse direction.

[paulV9CCG]

Dear @n8bot and @TrippyLighting,

Your care and help are greatly appreciated. This solved our problem and simplified the design work significantly.

[etfrench]

Depending on the complexity of the parts, it may be better to compensate for the anodizing in the CAM operations and not introduce changes in the model.  The Stock to Leave settings would control this.

It's too bad the CAM side isn't parametric, but you can use the Compare and Edit functionality to update multiple toolpaths and verify the settings.

[n8bot]

That does seem most sensible. Really, the only way to properly convey tolerance is with a drawing. If the CAM is made in conjunction with the model AND a drawing, then there should be no misunderstanding and all the CAM toolpaths will respect the needed tolerance. I.E.: 12.498 +0.0000/-0.0005 or whatever.