Tolerance in assemblies?

[renderedchild]

I did a search and didn't come up with much, so if I'm asking a FAQ, please point me in the right direction.

What is the best practice for sizing parts in an assembly?

Say you have 2 parts, one goes inside of another. Specifically in my case 2 sheet metal parts that get welded together.

In the past I have been designing the parts to fit together perfectly, then once the design is complete going back and shrinking down the parts to allow for tolerances. So the part that slips into another part gets undersized by .040" per side in the solidmodel and on my drawing the dimensions call out +/- .040".

In this most resent project I've been working on I have many layers of sheet metal that get welded and weldments that get welded to weldments and so on. As I started going through my normal process of shrinking parts I realized that what I was doing was A. a pain in the ass, and B. probably technically incorrect.

So that got me thinking, what is the correct(best) way to model parts with assembly tolerances in mind?

Should I model all parts to be the exact dimensions I want them, then in my drawing define my tolerances as +0 / -.040" or some such?

How do you handle this issue?

Thanks in advance.

 

[JMirisola]

I've always modeled the parts as they should fit together, then specified the tolerances in the drawing.
If you shrink your parts, then apply dims and tolerances you could end up with really undersized pieces, couldn't you?

Jeff Mirisola, CSWP, Certified DriveWorks AE

http://designsmarter.typepad.com/jeffs_blog

Follow me on Twitter

 

[CorBlimeyLimey]

First of all, there is no right or wrong way. Company standards often dictate the method used.

I usually use nominal (as opposed to median) sizes and apply the tolerances (e.g. H7-g6) in the models sketch dimensions. I then use Insert > Model Items (wherever possible) to apply the dimensions in the drawing.

 

[ctopher]

I also always model at nominal. Then I assembly the parts into assemblies as they would be in real world.
I create a drawing for each part and assy, then dim each one.
Tolerances are then applied, stacked, etc.
Finally I go back and adjust each part separately or within the assy to the desired tolerances.
It all depends on the design, materials, and specs.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[MadMango]

I would agree to always model your parts to nominal dimensions (vs median), along with adding your tolerances in the model sketch dims and inserting them from the model. I have also created configurations of min/max conditions, but this was mostly just for illustration or training purposes (pain to do).

 

[drawoh]

renderedchild,

If the mating parts are welded together, how are you going to inspect the interfacing dimensions? Is there any reason why you care?

On any manufacturing drawing, you should apply dimensions and tolerances to things that matter to you, and that you can inspect. Let your welder figure out how to assemble the two parts.

I strongly prefer to model to nominal dimensions, as noted above. Most of my stuff is machined. Some of it is sheet metal. I want to fiddle tolerances on my drawings. I do not want to have to fiddle the 3D[ ]model every time I change something.

The next time I design a casting, or any other part that goes out for rapid prototyping, I will model to the median dimensions. These guys like to work directly from the 3D[ ]model.

JHG

 

[Eltron]

Sounds like I part of the herd as well. It seems logical to me that you should model your parts as if they were manufactured perfectly and mate them up in the assembly accordingly. Then you can yell at the machine shops for not getting it right. After all, that's what tolerances are for.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[renderedchild]

Thanks for the advice guys.

To answer your questions:

JMirisola: Undersized parts is a concern as a result of undersized models and doing a blanket +/- .XX" tolerance. In the past I have noticed parts of a given weldment being undersized, but the over all dimensions always came out OK. I'm afraid in this particular project, with all of the stack up, that i wont get so lucky. With my previous logic if the parts are manufactured 100% correct per the drawing the parts will still be undersized.

drawoh: I wouldn't be inspecting interfacing dimensions necessarily, but as JMirisola suggested if parts get undersized and parts get welded to those undersized parts I could be dealing with a lot of tolerance stack up that would make the over all dimension that I do care about wrong. Granted this would technically be the welders problem if the final assy doesn't match the assy drawing, but why make their job harder? Welders have to fight parts moving around enough as it is under perfect conditions.

CorBlimeyLimey: Hey! that insert model items looks neat. I never noticed that before... I'll have to give that a shot. What do you mean here: "[...]and apply the tolerances (e.g. H7-g6) in the models sketch dimensions.", could you elaborate?


Thanks for your advice all, it sounds like I'm screwing myself a bit. Nominal models it is!

 

[JMirisola]

I'm not sure which version of SolidWorks you're using, but premium has TolXpert. It may help you out.

Jeff Mirisola, CSWP, Certified DriveWorks AE

http://designsmarter.typepad.com/jeffs_blog

Follow me on Twitter

 

[hendersdc]

If the parts can be manufactured within your stated tolerance and still be undersized for their function then you need to change your tolerance callout such that the parts will work if the manufacturer meets the tolerance. If the stack up is too big then you can use the RSS approach, counting on the fact that not all tolerances will be at their limits at once. Either way it sounds like you need to do a tolerance analysis.

Blanket tolerances are nice and easy to put on a drawing but it sounds like you will need some specific tolerance callouts to meet your needs.

 

[ctopher]

If you are sending your part files to CAM, it's better to model at nominal. This way the machinist can adjust to fit to the appropriate tolerances.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

 

[CorBlimeyLimey]

renderedchild,

Tolerances can be applied when dimensions are placed in the feature sketches.

In the Tolerance/Precision section of the Dimension Manager, various types of fits can be selected. Among those available are "Fit", "Fit with tolerance" and "Fit (tolerance only)". These use the standard notations for types of fit as described at

http://www.mitcalc.com/doc/tolerances/help/en/tolerancestxt.htm

Unfortunately some machine shops no longer recognise these fits, so I use the "Fit (tolerance only)" style which allows me to choose the type of fit I need, but only shows the resulting tolerance in the dimension.

I find them invaluable.

 

[MechEng2005]

I agree with Drawoh. Put your dimensions/tolerances on the weldment drawing for the after welding condition. It is quite possible to have an "incorrect" weldment based on proper parts.

For a simple example, assume a "H" shape was being made using 3 members. If it was critical that between the two vertical sections of the "H" were spaced at 36" apart, and I made the crossbar memeber 36" (+0, -0.02), I wouldn't necessarily expect the result to be what I wanted just by providing the pieces to a welder.

Also, I could (and often do) provide some "gap" built in. For example, I might give a welder the two vertical uprights and a piece 35 15/16" (+/- 1/32) long for the crossbar. With a properly dimensioned weldment drawing, the welder can lay the pieces out and shouldn't have any problem making the "H" with 36" exactly between the uprights, regardless of if the crossbar is actually 35 31/32" or 35 29/32".

-- MechEng2005