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How to resume a suppressed Feature by using relations?

MW_9726196
3-Visitor

How to resume a suppressed Feature by using relations?

Hi,
How can I resume an already suppressed feature by using relations? For example:

IF d12==100
ADD SUPPRESSED FEATURE
     INTERNAL FEATURE ID  570
     PARENTS = 410(#12) 1305(#17)

AND ADD

AND IF

 

If the feature is already suppressed and the equation (if d12==100) is true, the feature that gets added is in a suppressed state. How can I fix this?

Is there a conditional statment that removes "SUPPRESSED"?
Or is there a syntax in pro program that will regenerate automatically?



1 ACCEPTED SOLUTION

Accepted Solutions


@MW_9726196 wrote:

I understand Situation 1 and Situation 2. My Problem only occurs after Situation 2, when I change d1 to 100 again. 
After the feature has been suppressed from situation 2 (because d1 wasn't 100), I can't unsuppressed it again without doing it manually, even if d1 exactly is 100 again.
I am looking for a solution, so I can change from situation 2 to situation 1 and the feature "sketch 1" shows up without having to delete the word "suppressed" manually.


Hi,

1.] What Creo version do you use ?

2.] If you can, please pack your model into zip file and upload zip file.

3.] Before you start Pro/Program creation, the specific feature must not be suppressed

4.] See uploaded video (Creo 7.0.5.0)

 


Martin Hanák

View solution in original post

8 REPLIES 8


@MW_9726196 wrote:

Hi,
How can I resume an already suppressed feature by using relations? For example:

IF d12==100
ADD SUPPRESSED FEATURE
     INTERNAL FEATURE ID  570
     PARENTS = 410(#12) 1305(#17)

AND ADD

AND IF

 

If the feature is already suppressed and the equation (if d12==100) is true, the feature that gets added is in a suppressed state. How can I fix this?

Is there a conditional statment that removes "SUPPRESSED"?
Or is there a syntax in pro program that will regenerate automatically?




Hi,

you have to do it the other way around. That is, to resume a feature and turn it off using an IF statement.


Martin Hanák

Hi,
That's what I was originally doing: 

 

IF d12==100
ADD FEATURE
     INTERNAL FEATURE ID  570
     PARENTS = 410(#12) 1305(#17)

AND ADD

AND IF

 

But let's say, that in the first version d12 is not 100, the feature gets suppressed and it looks like this:

 

IF d12==100
ADD SUPPRESSED FEATURE
     INTERNAL FEATURE ID  570
     PARENTS = 410(#12) 1305(#17)

AND ADD

If now I want to use the second version where d12 is in fact 100, the feature that gets added is still suppressed. That's why I am looking for a statment that removes "suppressed" or would regenerate the feature into its original state (not suppressed).



pausob
17-Peridot
(To:MW_9726196)

You can't change the user-assigned suppressed/unsuppressed state with relations or pro/program.

Basically, if D12 is 100, then model will regenerate with feature ID570 suppressed.  you'll be able to unsuppress the feature manually.

If D12 is not 100, then the feature ID570 will show up in the model tree as suppressed, but you won't be able to interact with it.

Also, in your code, "AND"s should be "END"s, I think.

So I can only unsuppress the feature manually? Or is there another way to not "Add" a feature without suppressing it?
Let's say for example:

IF D12!=100

!ADD FEATURE

END IF

 

And you are right, it should bei "END" not "AND"..

Hi,

MartinHanak_1-1669406129629.png

situation no.1:

  • value of d1 is 100
  • Sketch 1 feature is visible

MartinHanak_2-1669406289557.png

situation no.2:

  • value of d1 is 99
  • Sketch 1 feature is not visible

Pro/PROGRAM contains:

 IF D1==100

     ADD FEATURE
     INTERNAL FEATURE ID  60
     PARENTS = 1(#1) 3(#2) 5(#3) 


 Sketch

  NO.     ELEMENT NAME     INFO                                                 
  ---     -------------    -------------                                        
   1      Feature Name     Defined                                              
   2      Section          Defined                                              
   2.1    Setup Plane      Defined                                              
   2.1.1  Sketching Plane  FRONT:F3(DATUM PLANE)                                
   2.1.2  View Direction   Side 1                                               
   2.1.3  Orientation      Right                                                
   2.1.4  Reference        RIGHT:F1(DATUM PLANE)                                
   2.2    Sketch           Defined                                              
   3       X-hatching      Closed curve sections will NOT be cross hatched      
   3.1     Display         NO                                                   

     SECTION NAME = Sketch 1 

    FEATURE IS IN LAYER(S) :
      03___PRT_ALL_CURVES - OPERATION = SHOWN

     FEATURE'S DIMENSIONS:
     d3 = (Displayed:) 50
          (   Stored:) 50.0 ( 0.01, -0.01 ) 
     d5 = (Displayed:) 100
          (   Stored:) 100.0 ( 0.01, -0.01 ) 
     END ADD
 END IF

 


Martin Hanák

I understand Situation 1 and Situation 2. My Problem only occurs after Situation 2, when I change d1 to 100 again. 
After the feature has been suppressed from situation 2 (because d1 wasn't 100), I can't unsuppressed it again without doing it manually, even if d1 exactly is 100 again.
I am looking for a solution, so I can change from situation 2 to situation 1 and the feature "sketch 1" shows up without having to delete the word "suppressed" manually.


@MW_9726196 wrote:

I understand Situation 1 and Situation 2. My Problem only occurs after Situation 2, when I change d1 to 100 again. 
After the feature has been suppressed from situation 2 (because d1 wasn't 100), I can't unsuppressed it again without doing it manually, even if d1 exactly is 100 again.
I am looking for a solution, so I can change from situation 2 to situation 1 and the feature "sketch 1" shows up without having to delete the word "suppressed" manually.


Hi,

1.] What Creo version do you use ?

2.] If you can, please pack your model into zip file and upload zip file.

3.] Before you start Pro/Program creation, the specific feature must not be suppressed

4.] See uploaded video (Creo 7.0.5.0)

 


Martin Hanák

Hi MartinHanak
I figured it out! The problem was, that the specific feature was suppressed, before I started Pro/Program and that's why I struggeled to unsuppress it.
Thanks for your help.

 

 

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