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  1. #1
    Join Date
    Jan 2019
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    Exclamation problem with formula

    Hi
    I just made some formula for some parameters
    i drawed a circle and i used constraint to set it's length. i right clicked on it and selected "edit formula"
    i selected my needed parameter and clicked ok. after that i saw no change !! the length of circle doesn't change after using parameter with formula ...
    Do you know what's the problem ?!
    ThanksUntitleddd.jpg
    Last edited by rezaafz; January 15th, 2019 at 04:04 PM.

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  2. #2
    Join Date
    Jul 2006
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    Default

    Make sure the parameter is for the radius of the circle. CATIA doesn't use diameters for circles!

  3. #3
    Join Date
    Jan 2019
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    7

    Default

    yes it's on radius but after selecting the parameter the circle length doesn't change ...

  4. #4
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    Jul 2006
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    OK, I'm not exactly sure how you are applying the parameter, so here are the steps you should be doing:

    1. double-click on the Radius dimension to edit the value

    2. right-click in the value field and select the Edit Parameter option

    3. the Formula Editor panel should appear

    4. in the Members column, select Renamed Parameters from the list. this will shorten the list on the right side to show only the parameters that you created.

    5. click the parameter you want to use for the Radius dimension, which will add it to the second line on the top.

    6. click OK to assign the parameter to the dimension. The dimension should change value.

    7. Exit the sketch and Update the part to the new radius value
    Last edited by MrCATIA; January 14th, 2019 at 08:41 PM.

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  5. #5
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    Jan 2019
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    thank you very much for whole response
    I do almost what you are telling me but still have the problem ...
    to see what's happening exactly , i recorded my problem , please watch this :

    https://drive.google.com/file/d/1IgA...ztnSko7BC/view

    Thanks

  6. #6
    Join Date
    Jul 2006
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    Thanks for the video, and showing us how you are applying the parameter to the dimension constraint. Everything looks good, until the end.

    I have a new question: What value is the Rp parameter set to? If it is set to 0, we just found the problem.

    Plus, I have a suggestion that I should have mentioned in my first reply:

    Your CATIA settings should to customized to show the parameters in the tree. First, go to Tools + Options + Infrastructure + Part Infrastructure, choose the Display page, and activate the Parameters option.
    parameter1.jpg

    Next, go to Tools + Options + General + Parameters and Measure, choose the Knowledge page, and in the Parameter Tree View section activate the With Value and With Formula options.
    parameter2.jpg

    Now there should be a branch in the tree with the Parameters and their values. Double-click on the Rp parameter and type-in a different radius value.

    Go back to the sketch with the circle and try to apply the parameter just like you did in the video. It should work now that the parameter is set to some length value. The dimension should also have a little ƒ symbol beside it indicating the value is from a formula. Edit the parameter in the tree again and set it back to it's original value (anything but zero).

    Here's a little shortcut:

    The next time you want to use a parameter to drive a dimension,

    1. double-click on the dimension to edit it

    2. type = and enter

    3. select the parameter directly in the tree
    Last edited by MrCATIA; January 16th, 2019 at 02:02 PM.

  7. #7
    Join Date
    Jan 2019
    Posts
    7

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    Oh my God i can't believe it! It worked !!!!!
    Thank you so much dear "MrCATIA" you really helped me a lot with your perfect response ... I really appreciate it

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