Any way to convert a part's system of units? 1

[acciardi]

Hello all...

We've been modeling in English units and have now been asked to start using metric in mid-stream. We have a few parts that have hundreds of hours into them, including detailed drawings.

Is there any way to convert them? All the parts are in TcEng, but I would be willing to take them out if needed to convert and then re-import them with new numbers if necessary.

Using NX 5.0.2.2.

Thanks!

Ed

 

[hudson888]

The short answer is NO but you can change drawing units much more easily that you might think.

Changing the part units is pretty much going to be more painful than it is really worth. The only method/s I know of require you to basically import each part into a file of the opposite units. In so doing assemblies are not re-built so it can become a rather disruptive process. Using Teamcenter simple adds an extra degree of difficulty to what is already a high-wire act.

Apart from the inevitable confusion and inconvenience that it may cause there are few real reasons for which NX as a program forces you to change modelling units. So by all means post back and let us know why you think that you really HAVE to do this.



Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[FrankMalone]

Hello,

What about ug_convert_part, this utility converts from in to mm and from mm to in. You must run a NX command prompt and execute ug_convert_part without arguments to see the available options.

About the drawings inside the parts it will be more difficult, the part will be in mm but the preferences in the drafting remain part based, so the dimensions the views etc. will remain with its values.

Frank.

 

[jerry1423]

I agree with Frank. It has been several years since I used ug_convert_part, but I assume that it is still available.

 

[acciardi]

Hi Hudson - thanks for the quick response.

The decision to go metric is pretty much an edict that I have no say in. We're a large company and all our suppliers are in the Far East and convert our drawings into metric anyway. IMHO, this should have been done 30 years ago. All my previous employers used metric.

It's just my luck that they decided to make the switch in the middle of my program.

I may be able to transition by doing the drafting on parts that have already been started using a metric template.

FrankMalone - I'll check out ug_convert_part - thanks.

Ed

 

[jerry1423]

If you go into "help" and enter "ug_convert_part" you will get something that should be able to help you.
I believe with ug_convert_part you can run a batch of files - so you can let it run overnight if you want.

 

[GBOLD]

Another option is to import the inch file into an empty metric file.

 

[acciardi]

GBOLD - thanks, but this didn't work for me. I created a new part using our metric template and did 'File/Import/Part' and NX told me to run ug_part_convert.

It may be because the part is in TeamCenter...?

 

[hudson888]

acciardi,

Where you're going to struggle with ug_part_convert is that I don't think that you can run it under teamcenter.

If you export all your stuff out of teamcenter and then convert it what occurs is that it uses the metric seed part which then no longer meets the requirements for teamcenter to re-import the data to the same item masters. It means that you'd need to manually reimport and link things back up again.

I'm not sure if having done this you're effectively able to rebuild the required links to all your assemblies using teamcenter, but in native they usually do need to be rebuilt.

It gets worse when you try to convert drawings since not only are they assemblies but a lot of information about the views etc. may be affected in the process. Certainly you would do well to test out a few of these different types of data in native first.

I could add that many people maintain other data like machining and motion data in teamcenter as well. Basically anything that you had with inter part, wave linked stuff in it or scaled units all risks being scrambled.

My advice is that unless you only have a few parts or the boss has more money than sense I wouldn't touch this with a barge pole. I would do the testing and estimate the time required to make the change then offer them the cost savings, since my feeling is that you lose little or nothing by leaving the bulk of data as is, or changing on a touch it fix it basis only when the next revision is called for.

The quick fix that might be enough to satisfy many people is simply to change the displayed units on the drawing dimensions. In that way you can have an inch unit CAD file and drawing but you can place metric units on the page. If you're not sure how to do that and wish to take the advice I'm offering then by all means post back, but you'll find the units settings under annotation style soon enough.

One other thing you might be happy to know is that you can work with a collection of metric and imperial parts together in any assembly at the same time. There are a few requirements to take extra care when you do so but the software is meant by design to allow that mode of operation.

When last we tackled this issue with a client we found that they had always set the selection colour of their imperial base parts to red as was the old UG standard. What we did then was to change the selection colour in the metric base parts to green so that as a site standard it was generally easy to discern one from the other. You can also include a units column in the ANT to help take care of this problem.



Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[acciardi]

Hudson -

You're just full of good news today

We currently do work with some mixed unit assys - metric fasteners in our english assemblies mostly. You can't make the odd item the work part, but one workaround I use is to drop the whole thing into a higher-level assembly that is metric. Then I can work in context on the oddball item.

I do understand that if I export/convert outside of TcEng I would have to re-import, but our system is configured to auto-assign legal part numbers, so it's not too bad if you understand how to use the Clone dialogue, which I do.

Not too thrilled about the prospect of losing wave links etc. As you suggest, I will try this on a few parts before I commit. Thankfully the re-parenting process has gotten much better in NX5 than it was in 4. Also, we keep a context assembly around for our Wave relationships, so it's usually pretty straightforward to re-link.

Thanks for all the help guys...

Ed

 

[joycejo]

I have a utility that I got from someone that works in windows to convert files. See attached.



John Joyce
Tata Technologies iKS
1675 Larimer St.
Denver, CO
www.myigetit.com

 

[JohnRBaker]

Be warned that if you use the 'ug_convert_part.exe' (which is still fully supported and which can be found in the UGII folder) it will ONLY convert the units of the Part file from either Inches to Millimeters, or Millimeters to Inches. All part models will be remain the same physical size as one would expect.

HOWEVER, any and all expressions created in the original model which had units, such as a Length parameter for some feature, will still be in the original units since the UNITS of an Expression is considered 'design intent'.

What this means is that if I had a feature with a block that was 100mm long and I converted the part to an Inch unit part, while the part file would now be considered an Inch native part file and any NEW objects created would be created using Inch units, the expression defining the length of the block would still be recorded as 100mm. Now that part would be the proper physical size, but the parameters defining it would be in their original units, in this case Metric. And before you think that this is not logical ask yourself what would you have expected us to do if while creating that original model, you had decided to create some length expressions in units other than Millimeters, say Centimeters, Meters and Kilometers, or for that matter, Feet and Miles?

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[Michael711]

John,

After converting a part with a Swoop surface from inch to mm,edit this surface using x-form funciton( with Associative Edit Freeform off), notice that previewed surface back to inch length. is the original expression taking effect?

Thanks,
Michael

 

[JohnRBaker]

What version of NX are you using? I just tried this with NX 6.0 and cannot see anything odd or unexpected in the results.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[JohnRBaker]

OK, now I see what you're talking about. I think I know what's happening and I'm going to open a PR.

BTW, the X-form has nothing to do with this since even if I attempt to edit the Swoop Surface itself the problem is apparent and in fact, the X-form actually 'saves' the expected size.

Anyway, if I learn anything, I'll pass it along.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[Michael711]

Thanks for your response..
I'm using NX7.0.0.3 protobuild.

Thanks,
Michael

 

[Michael711]

yes, I found that we can see that sams change when I edit the swoop surface.

thanks,
Michael