Best Practice UG/NX mixed units 2

[SDETERS]

What is the best practice of having parts that have mixed units in NX. We are using NX7.5. (We are coming from I-deas) We usually model all of our parts in inches. There is a new program here that may need to have all the parts modeled and 2d drawing in metric. I have done searches about not being able to set your work part in an assembly if you have mixed units. Is there other down falls using metric and inch models in an assembly? Also what other downstream issue like FEA ect. will not work well.

One possible solution we are thinking is to model the parts in inches and dimension it in metric.

 

[looslib]

Model in one unit and dimension in another is a real pain. How do you model 12mm plate, as .472441" or .5"? Since .5" is actually 12.7mm, do you dimension the drawing as 12.7, 12 or 13?

After that debate, then look at the asssembly and what the units do to your gaps when the components are mated.

The only drawback to mixed units is if your component oart is not in the same units as the assembly, you have to make it your display paart to modify it.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[SDETERS]

Thanks for the feedback.

We would model a 12mm plate at .472441. We would probably set up an expression to convert the mm to inch dimensions in the model. But it sounds like doing all of that is not necessary.

Thanks again

 

[JohnRBaker]

There's no need to convert values in the expression system since you can create Metric Expressions in Imperial parts or Imperial unit Expressions in a Metric part. So if you had a Imperial units part and you wished to create a features using Metric values simply go to...

Analysis -> Units lb - in

...and select 'kg - mm'. Now when you create a feature the dialogs and expressions will all default to Metric (mm) units. Note that the part model will still be considered an Imperial units part file in terms of the issue of Mixed-Unit assemblies, but at least you don't have to manually convert Inch to Millimeter dimensions. Note that the Units change in the analysis menu setting will only be remembered while you're working in that part file for that session only. Once you change parts or open another part the Analysis Menu setting will revert to the units of the Work Part.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[SDETERS]

Thanks for that feedback. This help many times over.

 

[looslib]

You can enter values in the other units when building your model, too. NX does the conversion for you.
If you have an imperial base part file and want to build a sheet metal part that is 12mm thick, just enter mm(12) for the thickness. Conversly, enter in(.5) in a metric part.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[SDETERS]

Sounds like we have many options. What would you suggest on how to handle the drawing? We are using the master Model approach to our drawings. Would you make the drawing a Metric. If we make the part imperial units? We want the drawing to have to metric dimensions only on it. Thanks for the feedback.

 

[looslib]

The drawing dimension would depend on where you are located. If in the USA, then most shops will understand imperial units better. If in Europe or Asia, then metric dimensions will be better.

If you are in the USA and do metric drawings, be prepared to pay more for the same part than if it was dimensioned in imperial units. I know it doesn't sound right, but reality sometimes comes at a cost.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[jerry1423]

Just a thought.
If working in master model . . . It is not an issue to have the model done in milimeters brought into the drawing file in inches, is it?
The only issue would be the threads, but that's an easy toggles - right?

 

[SDETERS]

Cool good information. We usually do all of our drawings in Inches. This is a special case where we want the drawing done in Metric. So we can start the part as imperial and do the "drawing" as a metric drawing. So the "part" units and "drawing" units do not need to match? Cool. Time to make some more drawing templates!

 

[JohnRBaker]

There nothing stopping you from creating Metric Unit Dimensions in a Imperial Unit Drawing file (you can even dimension in Feet and Inches if you're a mind to). Just go to Dimension Style preferences and change the Dimension units, so there's NO need to mess with mixed unit Part/Drawing files.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[mikebuchter]

We now have seeds that you can input in either inches or metric. We have it setup in expressions. UNITS ="English" or "Metric", Scale = IF (UNITS = "Metric") THEN (25.4) else (0). Every dimension must be divided by the scale.

 

[cowski]

Better change that to Scale = IF (UNITS = "Metric") THEN (25.4) else (1).

 

[JohnRBaker]

Every dimension must be divided by the scale.

PLEASE DO NOT USE THIS APPROACH TO SOLVE YOUR SO-CALLED MIXED-UNIT ISSUE!!!! Perhaps not today or even tomorrow, but I can assure you that one of these days you will wish you had never ever thought of doing this.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[looslib]

How to destroy the autoupdate of NX in one line!

Modifying every dimension in a file just to change units is asking for TROUBLE.

Like John said, one day it will bite you and it will not be pretty.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli