How to add parameter callout to sketcher pallete.

[Paul6]

Hi All,

What I am trying to acheive is to create a text string and symbol to be used as an item from the sketcher palette.

The scenario is this. 

I want be able to create sketch palette item which has a cavity number id reference # and the part number.

However when I create the sketch for this and want to add text, it does not give me the option to add the parameter it only gives a text option. If I add the parameter name in the text box and save this to the sketcher palette. When I call up this sketch from the sketcher palette in a part, I do not get the part number from the parameter in the model, I just get the text ( &part_number).

The part number is a parameter in my start part and subsequent modelled parts.

The only way I can get this to work is to insert this sketch from the palette and then edit the inserted sketch by selecting the parameter.

Is there a way to add the parameter to the sketch in the palette section, without the need to do a secondary edit.

Any suggestions welcome. Thanks.

I am using Creo 8.0.3.0.

[BrianMartin]

Hi Paul,

Try creating the sketch in a part model. It sounds like you're starting as a sketch - and therefore, the Use Parameter radio button is not available. Try the same thing in a sketch created in part mode, and the option will be there.

Once the sketch is created, you can save it from within the sketch interface. The resultant sketch (.sec) file will preserve the parameter. The file can now be included with your sketcher palette.

Good luck!

-Brian

[Paul6]

Hi Brian, 

Thanks for your reply, I have tried this approach, and the behaviour I am seeing is that saved sketch from within the part only holds the paramater value of that part in the sketch for the palette. So when I use that sketch from the palette for a new part the parameter value is shown of the old part ( where the .sec file was created). 

Again the only way I seem to be able to rectify this is a secondary edit to the inserted sketch from the palette and selecting the parameter radio button in stead of text.

[BrianMartin]

I have a few thoughts about ways to circumvent this behavior - one would be to utilize a UDF instead of the sketcher palette. Of course, I never like when someone fails to answer my question and suggests an alternative approach.

After looking at this for a bit, I'm convinced that once you save out the section, the parameter is simply lost and converts to "dumb" text. Under the circumstances, these less-attractive options may offer some benefit:

(1) using a user-defined feature (UDF) to load/p[ace your sketch

(2) using a mapkey which places the section and immediately updates the text to use the desired parameter

[Paul6]

Hi Brian,

Thanks for the prompt reply.

I have just tried creating a UDF from an existing text (parameter) engrave feature, but it has the same behaviour by inserting just the parameter value, when used in a new part. And it is not clear how I can move the UDF to a specific place on the new part.

It appears that I can only edit the UDF by disassociating the feature from the UDF and as before editing the text by means of the secondary modification to the feature,

If I am doing this as recommended, then this requires more work to locate and edit on the new part..

Thanks for your suggestion.

[BrianMartin]

Hi Paul...

I just created a UDF of a sketch in Creo 7.0 and was able to use the Ext. Symbols option in the UDF creation tool to select a parameter which updates with the placement of the UDF.  This approach works for me. 

UDF's are not easy - they are a bit of a dark art requiring some trial and error (and a lot of patience) to master. However, they are among the most powerful and critically overlooked features of Creo (IMHO).  There are many options and most are exceptionally poorly documented. The only way you get "good" at them is to spend lots of time playing with them until the options start to make sense.

I'll see if I can make one and submit it here to the forum as an example. Give me a little time to do this. Maybe it will give you enough of a starting point to modify it to your needs.

Thanks!
-Brian

[Paul6]

Hi Brian,

Thanks for the info. 

I am not overly familiar with UDF's and yes I would agree about the dark art associated to it.

I did try to recreate another one and was able to select variable dimensions to allow the placement of the UDF on the new part.

However I was unable to select a parameter or use the Ext.symbols option to add a parameter, but I think this is just my lack of experience and time spent using UDF's.

If you have the time  to create an example that would be great. 

Please let me know where you post it.

Thanks.

Paul.

[BrianMartin]

Hi Paul,

Try this... start with a solid piece of geometry. Place the UDF using 3 references (there are prompts):

1. Select a placement surface (intended to be a solid surface not a datum plane)

2. Select a vertical reference plane (this will provide a dimensioning reference left-to-right)

3. Select a horizontal reference plane (this will provide a dimensioning reference up-and-down)

The UDF is specifically looking for a parameter called "PART_NUMBER" so as long as your model has a parameter defined, the sketch text should reflect the parameter. If there is no such parameter, you'll see an error message at the bottom of the screen indicating that the last known value of the text has been used. 

Give this a try and see if it works for you. There are many of other ways to place a UDF. We could place it on a point, offset from a coordinate system... the possibilities are sort of endless and depend on what you're trying to achieve.

Thanks!

-Brian

[Paul6]

Hi Brian,

Thanks for the UDF. I can place this into various model files and it does call out the part_number parameter from the model into the imported sketch. I can then create the engrave feature from there. 

What I now need to figure out is how to actually create a new UDF to include the cavity ID sketch along with the parameter sketch and create the engrave feature. So that I have a complete UDF engrave feature. 

 i will have to get to grips with creating the UDF, calling out a parameter, still unsure on how to do this. Not a lot of info in the help files that I can find.

Thanks again Brian, its a good start to a work around.

Paul. 

[Chris3]

Create the features that you want in your part and then enter the UDF Library to create your UDF. It still uses the old Menu Manager even in Creo 11.

Click Create -> Give it a name -> Stand Alone -> No ref part ->  Select features -> Done -> Done -OK

There is lots more you can so. Selecting parameters to vary, naming the selections in a way your users will understand etc, but that is the basics.

[BrianMartin]

Hi Paul...

If you want to work together some time, I can block out some time to do a web meeting (Teams, Zoom, GoToMeeting, etc). You can probably do your entire engrave feature as a UDF and save yourself a ton of time.

Thanks!

-Brian

[Paul6]

Hi Brian,

Thanks for the offer of a web meeting that would be really helpful if you have the time.

Not sure how we can set this up.

FYI. I am based in the UK.

Thanks

Paul. 

[vnamboodheri]

Hello @Paul6, 

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