ISO Standard Fits and Tolerances

[ptc-2151062]

Hello all,

We have recently decided to use ISO Standard Fits for hole/shaft dimensions, such as a hole dimension 40H8. This has created confusion with some of our vendors. Also, for example, when +/+ (or -/-) tolerances are used for a hole on a drawing, the hole in the solid model is now outside the actual tolerance range. This could be problematic if a vendor typically makes parts based on the solid model, and uses the drawing to verify the part.

My solution is to show both the ISO tolerance callout (ie H8), as well adding the actual tolerance in parentheses, such as 40H8 (40.039/40.000).

Any ideas on how to do this in WF 5? The problem is getting the parentheses into the callout.

Thanks,

Andri

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[s.iyer]

To get a similar effect, set the following...

Config.pro options:

tol_display --> yes

tol_mode --> Nominal

Tolerance_Class --> medium

Tolerance_Standard --> ISO

-----------

File --> Properties --> Change Tolerance --> Retrive Tolerance --> Hole "H", Shaft "j" and "g" [Alternatively you may retrive commonly used tolerance Grades in you START.prt]

------------

Config.dtl option:

tol_display: YES

Tolerance mode: LIMITS to get the upper and lower limits as shown for 60 H7 and Tolerance model Plus/minus to get the result as shown for 80 j7.

******************

As for the vendor using the solid model for reference, you may choose to use DIMBOUND. Dimbound binds the size to either the upper limit or the lower limit or at the Central portion. e.g. For 60 H7, if you bind the geometry to the Central, it would bind the geometry to 60.015 and not 60; meaning your measured diameter would be 60.015 which is the average of 60.000 and 60.030.

[ptc-2151062]

SCIYER26,

the outline you described is exactly what I was looking for. I was not aware of ISO Tolerance tables built into ProE. However, I'm still not getting the results shown in your drawing. I have set all the config.pro and config.dtl options, and I can retrieve the H tolerance (For WF5, it's File-->Tolerance Standard-->Tol Tables-->Retrive--> Hole "H". At this point, I regenerate, but nothing happens to my dimensions. Is there an additional step I am missing here? How do I apply the H7 tolerance to a specific dimension?

Also, you talked about DIMBOUND. Is that a config.pro option? How do I use it?

Thanks for your help so far,

Andri

[ptc-2151062]

Ok, I figured it out. I was trying to retrieve the ISO tolerance Tables in drawing mode, instead of in the 3D model. Once the appropriate tolerance table has been retrieved, it can be accessed in the drawing in the dimension properties window. I've also tried it with inch drawings, and the ISO tolerance is correctly converted from metric. Awesome!

Also, the DIMBOUND command is found in the 3D model under Analysis-->Dimension Boundaries. Here you can set the boundaries to either Upper, Lower, Middle or Nominal. This works great.

The only problem now is the decimal places. If I want to show the following: 0.75 H7 (0.7508/0.7500), I should be able to do that by setting the nominal decimal places to 2, and the unchecking the "default" box for the tolerance decimal places and setting it to 4. However, when I regenerate the drawing, the tolerance decimal places goes back to 2. This only seems to happen when I set the DIMBOUND to something other than Nominal. Any ideas what might be causing that?

Andri

[s.iyer]

Try setting the config.pro option: "default_dec_places" to 4 and save the config.pro.