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| Forum Highlight: CATIA V6 |
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| Author |
Messages |
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COE-FORUM-USER
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| 02 May 2006 01:09 AM |
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Hi All
I wonder if somebody come across similar problem
I Build a rule in Knowledge Adviser to Activate and
Deactivate Pockets from a Pad
I change that rule so it will do the some operation with
Cut out in sheetmetal parts
I have following problem
Rule will deactivate sketch of this particular cut out
But not the Cut Out .
Instead I have strange errors
Can you help me to find a solution
Thanks
My Rule
/*Rule created by Les */
if (VV == "right")
{
`PartBody\Cut Out.13\Activity` = true
Message("Light are on")
}
else
{
`PartBody\Cut Out.13\Activity` =false
}
----------------
Catia V5 r14 sp6
Best Regards,
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BPRASAD
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| 02 May 2006 09:25 AM |
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Hi Les:
Here are some tips. Occasionally, the feature of the part you are trying to deactivate are required for building the part. As a result, you may be getting errors since the two features are dependent on each other. If one vanishes the others cannot co-exist.
1. I have avoided the dependentcy, by creating a sketch on a separate datum plane at the same location as the original face -- rather than using the "face of the solid-feature (say Pad) or similar intrinsic faces" to create the pocket.
2. You may first want to try doing it (activate/deactivate) interactively. Can you activate and deactivate the features without any hick-ups OK? If you could do it interactively, you should be eable to do it also via KWA rule as well.
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Brian Prasad
COE-DPC/KBE Chairperson |
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COE-FORUM-USER
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| 03 May 2006 12:40 AM |
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Hi Brian,
This is the error message :
Build of Cut Out Left.1 failed.
An unexpected error occurred during the build.
--------------------------------------
Thank for the tip
I have done this before, sketched on planes not on the faces.
I delete this cut out and create new one with the some name
I’m not able to explain why ,but all is back to normal.
Brain I hope I can ask for advice
I’m trying to write a rule in KWA
To put limits on a parameter
Standard Value of Parameter Length.1 =500mm
Limits are min 450mm max 550mm
What I need is a Rule
If Length.1 > 550mm
And Length.1 < 450mm
Then Length.1 = 500mm
I’m having problem to achieve that in KWA rule
Can you suggest something
Thanks,
Regards,
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CLIFFJOHNSON
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| 03 May 2006 10:30 AM |
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You can't do that in a Rule. CATIA considers it a "loop".
Of course you know you can simply define a range on the parameter iteself:
1. Double-click parameter
2. Right click on value
3. Select "Add Range..."
If you want to do what you are proposing using KWA tools you can use a Reaction to do it.
1. Make the reaction fire on Value-Changed for your parameter
2. Use syntax like this: if Length.1 > 10mm or Length.1 < 0mm { Length.1 = 5mm }
HTH,
Cliff |
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COE-FORUM-USER
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| 03 May 2006 09:10 PM |
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Thanks Cliff,
This is excellent.
In the meantime
I have tried KWE for few minutes
But looks like the variable you need to declare
Is for all Hole or Pads……
We received KWE Lic recently.
Would it that be easier to do that in KWE ?
Thanks for your Help
Best Regards,
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