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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.
Solved! Go to 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.
Randy,
can you upload your model and provide parameter name, you want to create ?
Martin Hanak
I emailed the file to you. I do not see an attachment icon in this window.
You can attach files using the advanced editor... upper right corner of the reply UI.
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
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?
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.
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.
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.
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
You are welcome
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
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
How can you view current relations? I have a different working model with relations but I can not view them.
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.
Nice trick!