Defualt imperial units remains after config.pro changed to metric

[Fulvia]

I am using Creo Parametric 6.0.6.0 Student. I have set up the config.pro file with all my preferences which includes metric units. 

When I open a model the units are Imperial but all my other preferences are correct. 

It's a bind having to remember to change it for every new part.

Is there a fix?

[KenFarley]

It is uncertain what you have set up in your config.pro, or whether that file is even being read when you start up Creo. The config.pro is read from the working directory - when you start up Creo the working directory is set to the "Start In" directory specified by whatever shortcut you use to start Creo. If you start up Creo by double clicking on a file in a directory listing, it is likely you are not having your settings applied. Creo will start up with that file loaded into memory and in the directory in which that file resides.

If you are opening an existing file, no matter what you specify in your config.pro, that file will remain with whatever units it has, unless you explicitly change it for that file. The config.pro settings  only apply to new files.

In case you might be missing one, here are the config.pro settings I have to set the units.

pro_unit_length    unit_inch
pro_unit_mass      unit_pound
pro_unit_sys       ips

Lastly, probably the best way to ensure the units you want are applied to new parts is to set up "start parts", which are simple part or assembly files with all the correct settings you want (units, material, etc.) Put them in a directory and reference this in your config.pro with the "start_model_dir" setting. My entry, for example, is

start_model_dir c:\ptc\Templates

Hopefully with the student version you will be able to set these types of things up.

[Fulvia]

This is my Config.pro file. Creo is definitely picking it up as all the other changes I have made are working. I will need more information on how to set "start parts"

[KenFarley]

You could just search for "start parts" and you'd find lots of discussions of the topic as well as advice about how to go about it. Stuff like:

https://community.ptc.com/t5/3D-Part-Assembly-Design/Start-Parts/td-p/402183 

[Fulvia]

I can't find anything in the "start parts" discussion on setting unit systems. Can you be more specific?

If the metric units are specified in the configuration editor a new part should start in that system, especially when all the other items in the ile are correct.

[tbraxton]

The units are saved in the part files you can have start parts with different units (with unique names). Create your part and save it the start part path, you will then have access to it any time you create a new part.

Watch this video:

https://www.youtube.com/watch?v=43ElkU46erk&t=20s 

[MartinHanak]

Hi,

you can use simple procedure to create your start part.

• create new empty part (do not use template) ... give it mystartpart name
• set units
• create basic datum features
• save

How to use it?

• open mystartpart.prt
• use Save a Copy command to create new_real_part
• erase mystartpart.prt
• open new_real_part.prt and build its geometry

[Fulvia]

I assume for every part I created I would have to start by opening mypartstart.prt every time and then create a copy as my new part. This will be as much hassle as changing the units using the prepare command.

[MartinHanak]

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@Fulvia wrote:

I assume for every part I created I would have to start by opening mypartstart.prt every time and then create a copy as my new part. This will be as much hassle as changing the units using the prepare command.

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Hi,

if you add following option into config.pro then you are done

template_solidpart absolute_path_to_your_mypartstart.prt

[Fulvia]

This is working if the mmns_part_solid is selected.

How do I make this the default?

[MartinHanak · Accepted solution]

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@Fulvia wrote:

This is working if the mmns_part_solid is selected.

How do I make this the default?

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Hi,

use option similar to the following one

template_solidpart E:\PTC\Creo6_051\Creo 6.0.5.1\Common Files\templates\mmns_part_solid.prt

Also you can copy mmns_part_solid.prt to your own directory and use corresponding path.