How to Clear CREO 2.0 Parameter Names

[ptc-4175781]

I used parameter names (tools/parameters) to set up the model to be parametric with ANSYS Workbench. I am creating a new model and want to use the same parameter names as another model. I started a new session of CREO 2.0, created a new part, named the dimensions and then when I tried to create the parameter, I got a message that the Parameter name was already in session.

How do you clear parameter names? The old names do not show up in the Parameter List.

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[MartinHanak]

Randy,

can you upload your model and provide parameter name, you want to create ?

Martin Hanak

[ptc-4175781]

I emailed the file to you. I do not see an attachment icon in this window.

[TomD.inPDX]

You can attach files using the advanced editor... upper right corner of the reply UI.

[ptc-4175781]

OK. Thanks for the note.

[ptc-4175781]

I figued it out. I was naming the dimension the same thing as the parameter which CREO will not allow.

Example of correct way.

Name dimension: insert_od

Name parameter: ds_insert_od.

Then all is OK.

Now I need to figure out what I am doing wrong with creating the relations:

insert_od=ds_insert_od

I keep getting the error message: Unitless value assignment for symbol ‘D20’.

I followed this method to create the relation:

I clicked on relations icon.

Then, clicked on the dimension with the named dimension.

Then, clicked the “=” sign.

Then, clicked Insert from list and chose the parameter and ended up with:

insert_od=DS_INSERT_OD

[TomD.inPDX]

I am able to add the relation to the model without an error mesaage. Creo 2.0 M040 in the attached file.

Remove the realtion and find the insert_od parameter and remove it. Then try again from the relation UI.

"insert_od=ds_insert_od"

I have seen this issue reported before and PTC support fixed the file. But in your case, I don't have trouble getting this to work. What version are you running?

[TomD.inPDX]

And when I re-read your post... if I 1st change the ds_insert_od to insert_od

are you then trying to add the "insert_od=ds_insert_od"? You probably have to declare ds_insert_od first.

relations

ds_insert_od=7.861

insert_od=ds_insert_od

Once this parameter is created, you can remove the 1st line from relations.

[ptc-4175781]

I tried your suggestion to no avail.

ds_insert_od=7.861

insert_od=ds_insert_od

error Unitless value assignment for symbol 'D13'.

I attached the revised model.

[TomD.inPDX · Accepted solution]

I am going to suggest this is a version issue.

In this file you already changed the dim symbol to insert_id

and you created the unitless parameter ds_insert_od.

I open relation and add insert_od=ds_insert_od and check the relations.

I get a successful message.

Do you have maintenance? Again, I think this is a known issue but if you can, report it.

Video Link : 5265

[ptc-4175781]

Wow. Nice video to explain your steps. I agree it is probably a software issue. It may be the way our IT folks configure the system.

Thanks for all of the support. You have been a great help.

Randy

[TomD.inPDX]

You are welcome

[MartinHanak]

Randy,

I opened your thesis_insert_v2.prt in Creo Parametric 2.0 M100 and added the following relation successfully

insert_od=DS_INSERT_OD

So M100 is OK. Test the problem without config.pro.

Martin Hanak

[ptc-4175781]

As suspected, our CAE Team changed a setting that caused the problem. To fix: Go to Relations/Utilities and uncheck the Unit Sensitve box.

Thanks to all for the support.

Randy

[ptc-4175781]

How can you view current relations? I have a different working model with relations but I can not view them.

[TomD.inPDX]

They get mushed all over the place. A quick place is to show the Program dialog.

Model tab>model intent>Program>show design. In the top it shows all relations... but not all parameters.

[ptc-4175781]

Nice trick!