Best practice plastic parts offset design

[Anonymous]

I wonder, is there a "best practice" method how one can design plastic part fits without manually design the offset into the Feature/Part itself? For instance, if i create a multi-solid part with plastic features like lips, etc., the dimensions are exact without offsets. But for 3D Print for instance (i think its the same for mold), i need certain offsets to let the parts fit. How can I achieve this without design the offset into the part itself but design it exact to use multi-solid parts but in the output print it will respect for instance a 0,2mm fit offset for a lip?

I am refering to this howto video: https://www.youtube.com/watch?v=pT0rcAvTTwE especially the lip part but also the boss features will not respect offsets, these commands use always exact dimensions.

For Metal, I think it is the same.

Thanks for your reccomendations and input!

[JDMather]

Do you have an example parts(s)?

I always teach my students to build real world clearances into their parts.

[mcgyvr]

Using the lip tool you have full control over the dimensions of the lip..

Like anything else its up to the part designer to model the part with any tolerances/offsets/clearance areas,etc.. as needed..

[Anonymous]

I can not believe this is the prefered practical solution. With different material outputs you have to model the part dimensions differently for every production technology??

So If you want to create a molded part including tool design but rapid prototype it with for instance 3D printing using FFF, or output it for different formats for example FFF, SLS, STL or even wood modelling, you always have to change the source parts dimensions - because the different processes require different tolerances?

That I can not believe, there must be a better way to adapt for different production processes. Is there any way to include the tolerance system of inventor in the design process?

Thx,

Mike

[JDMather]

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@Anonymous wrote:

...in the design process?...

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I don't understand the question?  That is the process being described here.

[mcgyvr]

I understand where you are going.. for the most part..

Its just not something that Inventor (nor any other CAD program AFAIK) does..

You've got your head too far in the "future" 

One uses tolerances to ensure proper fit in the end production product..

Not to adapt to the inconsistency of multiple prototype processes/machines..

But the abilty to say (for example) scale all holes by 1.2% and internal vertical surfaces by 2% inward,etc...because you know your 3d printer will always "flow" a bit would be interesting.. But even so.. hole to hole and location to location that scale factor might not be the same at all.. Even FDM machine to FDM machine will be different based on the machines physical capabilities..melt temperatures..materials used,etc..

[Curtis_Waguespack · Accepted solution]

Hi michaelruepp,

If you anticipate the need to have this "offset" value change, and it is consistent (or mostly consistent) you could define a parameter and simply reference that in the model's lip features. Then should it need to change, you can simple change it from the parameters editor and have all of your other dimension equations update.

So for instance you might add a Lip_Offset parameter to a list such as in this example. And then when you define the Lip feature instead of leaving the offsets at 0mm, for example, you simply reference the Lip_Offset parameter.

Make the Lip_Offset parameter a multi-value parameter tied to a material ( using iLogic) and then you can update the offset value quickly for different prototyping, until you decide on the final material.

Excerpted from the Mastering Autodesk Inventor book

I

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[Anonymous]

Thanks for your input, but actually one not only use tolerances to define fittings (ISO H6/7,etc.) but indirectly also for defining machining/tooling decisions, so some tolerances wouldn´t be practical to achive with this tool, so you have to use another (like milling vs. spark erosion) - subsequently the tolerances chosen will have an effect on what process/machine/tool you will use to create the tool. So you can never achive a H7 fitting with a FFF 3D printer so it makes no sense to use this tolerance in combination with this process, and so on...

What you wrote at the end is exactly what I thought about, that the Software detects somehow the mating features of the parts and adapts it to the material/process to achieve overall dimensions, especially in the multi-solid to derived assembly workflow where it is quite unhandy to manage the offsets because all you get is a bunch of grounded parts in the iam.

Thanks, Mike!

[mcgyvr]

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@Anonymous wrote:

Thanks for your input, but actually one not only use tolerances to define fittings (ISO H6/7,etc.) but indirectly also for defining machining/tooling decisions, so some tolerances wouldn´t be practical to achive with this tool, so you have to use another (like milling vs. spark erosion) - subsequently the tolerances chosen will have an effect on what process/machine/tool you will use to create the tool. So you can never achive a H7 fitting with a FFF 3D printer so it makes no sense to use this tolerance in combination with this process, and so on...

What you wrote at the end is exactly what I thought about, that the Software detects somehow the mating features of the parts and adapts it to the material/process to achieve overall dimensions, especially in the multi-solid to derived assembly workflow where it is quite unhandy to manage the offsets because all you get is a bunch of grounded parts in the iam.

Thanks, Mike!

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Yes.. In general you design the tolerances based on the product/parts needs and then you pick an appropriate way to produce those based on those stated tolerances..

So yes having super tight tolerances makes no sense if you are sending a part for 3d printing..

So far I've NEVER nor will I ever produce a special drawing for a machine/process specific prototype.. I will do the "production ready" drawing and all my prototype suppliers are well aware that we won't "ding" them if a 3d printed part or whatever doesn't meet the drawings "production ready" tolerances..

To go along with what Curtis wrote above.. Which is a great solution too..

I think if I had the need to have these differences and an actual model along with them I would probably use an ipart..Then one "member" would be "production ready" and another would be "prototype ready" where I could adjust dimensions to fit the manufacturing process be it 3d printers or whatever..

Or even just 2 drawings.. One uses the "parts tolerances" automatically and another where you simply enter another tolerance suited to the "less accurate" proto process..

To me what you are saying is interesting but I see that ability to be very complex to implement the "easy button" on that and really only be needed for a small audience.. 

There is the "inventor ideastation" where you could post your suggestion and see how it goes.. Being that 3d printing and other new technologies are becoming more mainstream it might be something for them to look at now..

[Anonymous]

Yeah the easy button will be hard to implement, but thinking about industry 4.0 and whatnot, complete streamlining of the prototyping/machining process without human intervention, there must be some output profiling in the design process somehow in future Software i guess, wheter it be in the CAD or machine software... Regards, Mike