Creo Version In Parameter

[llie]

Does anyone know of a way to automatically show the Creo version (3, 4, 5, 6, 7,...) as a parameter?

We implemented the values in param values list, but that is a manual step for the users to change when we go to a new version. We also have it set in our start parts as well as our Windchill templates, but that is a change we will have to do every time we go to a new version. 

We are trying to be in compliance to ASME Y14.47 and  14.41

[tbraxton]

I am pretty sure you will have to use one of the API programming tools (toolkit, Jlink etc.) to automate this. Unless it has been added in Creo 7+ an internal parameter accessible by the UI for the software version has not been available previously.

[llie]

I even tried this PTC article without an success in Creo 7.0.4.0

https://www.ptc.com/en/support/article/CS352759

How to create a parameter with value as result of check "PRO_VERSION" in ModelCHECK

I guess it is time to open a PTC case.

[Mahesh_Sharma]

Hi @llie 

TO make it working, ADD_CHK_PARAM in appropriate check file needs to set as Y and in respective start file add PRT_ADD_CHK_PARAM VERSION PRO_VERSION

Thanks 

[llie]

Mahesh,

I have tried what you suggested and it still does not work. I will open a PTC ticket and see if someone can see what I am doing wrong. 

[Mahesh_Sharma]

You can submit a TS case to get this working. 

For a quick review, share the overview details in ModelCHECK report and check, start file. 

[TPWitt]

We also are working to comply with ASME Y14.47 and ASME Y14.41. We have notes that pick up the Creo version. If a parameter is added and Creo 7 is placed in the parameter. The model is later edited in Creo 8 and modelcheck is run it would not alert you that the parameter is out of date. I would like to see an active parameter in Creo like PTC_MASTER_MATERIAL and PTC_REPORTED_MATERIAL.

If PTC could add something to the encoded settings like PTC_CREO_VERSION. Then we could have a note that reads

SOFTWARE APPLICATION: Creo 7 (or 7.0.2.0)

and when brought up in Creo 8 would instantly update to SOFTWARE APPLICATION: Creo 8 (or 8.0.1.0)

[BenLoosli]

When I follow the steps in that CS article, it adds the Version parameter, but the value loaded is ERROR.

I am doing this in Creo 7.0.7.0.

Material is set, so that 0 is also an error, but for another thread.

ADD_CHK_PARAM

Number of parameters added or updated for MC check information: 4

Parameter	Value
MATERIAL	0
UNITS_LENGTH	INCH
MODEL_NAME	W14X30_BEAM_ANGLE_BEAM_11.PRT
VERSION	ERROR

[llie]

Ben,

I am also getting the Error output for Version. I did open a PTC case and submitting my ModelCheck files to them. 

[BenLoosli]

I tested it in Creo 4 M080 and get the same results.

Seems it has been broken for a while.

[Mahesh_Sharma]

Hi @BenLoosli 

You may try creating a new part > Save and run ModelCHECK, share the results. If possible in standalone session of Creo Parametric. 

Thanks  

[BenLoosli]

Running without having Windchill connected (offline) the Version parameter is created and populated with: 3800 2021424 [7.0.7.0]. My test file is in my Working Directory which is not in Windchill.

Closing the file and erase, connect to Windchill and open the same test part, now it gives the Version data.

Close Creo and restart it with Windchill and the same test file creates the Version parameter with version data.

Create a new file and the Version comes back with Error in the same session of Creo.

So the question is: What is Windchill connectivity have to do with the file version and the ability to read a Creo parameter?

[llie]

Ben,

Thanks for testing as well. We mainly run Creo connected to Windchill, so having our users disconnect to get a parameter to populate would never work at Raytheon. 

That was my question I was going to ask Mahesh, what does Windchill have to do with it not populating correctly?

[Mahesh_Sharma · Accepted solution]

Hi @BenLoosli 

Set the config MC_GET_VERSION_FROM_META_DATA YN Y in config_init.mc and test the issue. After setting this I am getting the values correctly. 

Thanks. 

[llie]

Ben,

Mahesh and I  got mine to work with Windchill being active. 

Thank you Mahesh.

[BenLoosli]

It works....sort of!

When I did the testing yesterday without Windchill, I got this for version: 3800 2021424 [7.0.7.0]

Adding the setting and running it with Windchill, I get this: 3800 2021424

Setting Windchill to offline and opening the file fresh, I still get: 3800 2021424

Commenting out the setting and restarting Creo offline, I get: 3800 2021424 [7.0.7.0]

What happened to the release information?

[BenLoosli]

Are there any plans to include the version name [7.0.7.0] as I have shown in the prior note with Creo offline from Windchill?

The users have no idea what 3800 means and even less so about 2021424.

It would be nicer if the Version parameter only showed [7.0.7.0] and not 3800 2021424.

I do know what the codes mean, but most users do not.

We could write relations that translated 3800 2021424 to [7.0.7.0] but that takes editing files and would only work for new files, not existing files saved in a newer version.

[llie]

@BenLoosli I so agree that the user has no idea what 3800 20211424 equates to in Creo version. We ended up using the params_values.lst and setting it in our start files to the correct value, but that means we have to re-release new start parts each Creo version that we move to, which does have its benefits, but is a pain.

[BenLoosli]

When I follow the steps in that CS article, it adds the Version parameter, but the value loaded is ERROR.

I am doing this in Creo 7.0.7.0.

Material is set, so that 0 is also an error, but for another thread.

ADD_CHK_PARAM

Number of parameters added or updated for MC check information: 4

Parameter	Value
MATERIAL	0
UNITS_LENGTH	INCH
MODEL_NAME	W14X30_BEAM_ANGLE_BEAM_11.PRT
VERSION	ERROR