Simply delete a user created parameter

[NG_10722318]

For some reason I am not getting an option to be allowed to delete this parameter (which I created like 3 minutes before). Creo can be awfully difficult in the way it handles options and I for the life of me cant figure it out after much googling and searching.

Any idea what "I" am doing wrong?

[IbrahimTayyab]

I am not sure but it seems to me that happens when the parameter is being referenced by something else for example a dimension is using the parameter as a relation, try right clicking the parameter and go to info-> where used. Does it show it being used somewhere?

[NG_10722318]

Right thats likely it its saying it is used as one of the dimensions but i deleted it when I changed the parameter name (created a new one) and there is no longer a dimension in the drawing but its obviously stored somewhere. 

How do I find a list of dimensions in the drawing and delete the one its attached to?

[NG_10722318]

You can see its attached to something but its not driving anything. The sd4 is a ghost literally not being used by anything.

Is there a way to see a FULL list of these "sd4" dimensions being auto created?

[NG_10722318]

People may not be understanding what i am asking so i grabbed a screenshot from inventor... Its in the literally same "parameters" area. Except instead of hiding all the dimensions (so someone can actually use and view them) Inventor has them all on display so you can rename them, change them, all sorts of things (you can also VERY easily export them which after much googling seems to be a MUCH requested option for creo)

In short I am trying to get this info in CREO so i can fix the broken dimension

[IbrahimTayyab]

I'm not even gonna lie I came across the same issue when I tried replication your problem this morning; we'll both have to wait for someone with more experience 😂

Although I say that deleting the feature with the relation did allow me to delete the parameter, (a sketch with multiple shapes in my case) later on however of  course this is not a satisfactory solution.

[NG_10722318]

Lmfao ... welp .. that oddly helps 🙂 

It has something to do with the way I deleted the dimension i know that. But it seems odd there is no alternative reference we can access to get at the danged thing. 

Is it "possible" to re dimension something using the same dimension number "sd4" then re-delete it correctly? in essence redefine "sd4" as say 12mm or something. This should unlock the variable?

[IbrahimTayyab]

Part 1/2

I think I got it, seems like an easy fix. I'll run you down through the whole process.

I create a parameter called x with a value of a 5 in a fresh part.

I make the diameter (sd0) of a circle equal x.

Now I decide I don't the diameter to be equal to x and then click the dimension in sketch feature and delete it It changes colour from black to blue.

I click ok in the sketch and go to my parameters and I find that I can not delete parameter x even though it seems nothing is being referenced by it.

I right click and find it is still being used in the sketch.

Now the issue is that the relationship still exists even though the dimension sd0 does not, to prove this I go into relations and voila it is still showing sd0 = x.

I can just erase that statement and then click verify and now as you can see I am able to delete parameter x.

[IbrahimTayyab · Accepted solution]

Part 2/2

To recap there is a way to get relations in selected features that is "look in" and then selecting the feature where the parameter is being used.

I figured the best way to avoid this issue is instead of deleting the dimension with the relation it is best to change it.

For example, I have created a new parameter y with a value of 5 again and made sd1 equal it. (Note that the diameter is now sd1 instead of sd0 since sd0 was deleted previously)

Instead of deleting said dimension to change the value I will go into relations and change the value of the dimension there so that it is not equal to y anymore.

I set the value to 22 and verify the relations, the circle now has dia 22 and parameter y is not being used anywhere else and I am free to delete it.

I have made it a bit tedious but I hope it was helpful. Let me know if you have any problems.
Best regards,
Ibrahim

[NG_10722318]

Well done 5 stars!

I didnt really understand what you meant by "Relations" so in case someone else is looking,

Relations is a whole other button to parameters (2 down on the ribbon)

Thing is you MUST be in the sketch where it was originally done to show up in the relations list. You cant just go there while in model view or it wont show up. This tipped me up for a number of minutes before "editing" the sketch and THEN opening up relations.

But after doing this solution I was indeed able to delete the parameter causing me issues. 

[IbrahimTayyab]

I recorded a short video of the "relations" tab in case it might be helpful. Note that I used look in "section" and then selected the sketch later I showed that the parameter y was being used in the same section just for your information. The mp4 attachment will load quicker btw

[KenFarley]

What you're seeing is the reason I never use relations in a sketch. When I first started using relations to govern geometry I would use them in sketches. However, later, when I wanted to adjust things, I found that the opaque nature of sketch relations was making it really hard for me to track down what is locking parameters, etc.

As a result of some really messy detective sessions I long ago resolved to only use model based relations. Especially if I'm using parameters in the calculations.

Also, a big help to anyone in the future who might be looking at what the relations do (especially me) is to rename any dimensions I'm using in them. Give them a name that makes sense. "d1127" doesn't mean anything, but "diaOuter" is very helpful. I've seen some models with many many relations that just use dimensions of the "dXXXX" format and it makes you want to just shut everything down and go home.

[kdirth]

You can get to any relation without entering into a feature.  The key is to select the correct type of feature in the Look In drop down menu then select the feature in the tree.