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SK_RD81-Visitor
1-Visitor
November 17, 2021
Solved

Extrude numbers from 1 - 10 helical on a surface

  • November 17, 2021
  • 5 replies
  • 3666 views

Hi,

Can some one help me how do you extrude a scale on a cylindrical part with the numbers from 1 to 10 the easiest way. The only option i have found so far is making a lot of planes and extrude the numbers individual.

 

I am seeking a smarter way to do it, because i need to do it with many more numbers

 

 

Best answer by LukaszMazur

Check my attached model if that's something you want to achieve. I've made it to see if that's possible, so I haven't investigated much why it's considered not regenerated 😉 Model is made in Creo 4.0, BTW.

See sketch relations for the first group in the pattern: there is a relation that sets the number in sketch text to the dimension of sketch point (and converts it to string, as patterning the dimension kept changing the parameter type to real number and it was displayed with many decimal places ;)).

Pattern is used to drive sketch location (sketch text is attached to the datum point on the curve) and incrementing the numbering parameter.

5 replies

K
KenFarley21-Topaz II
21-Topaz II
November 17, 2021

A part of the problem can be addressed, perhaps, by using the methods outlined in the following:

 

How to pattern text where the text string is incremented for each pattern member in Creo Parametric 

 

I've had situations (linear scales on sliding parts, angular damper position indicators, etc.) where this type of thing would have been nice, but I just used a "dumb" sketch. Not easily adjustable, tedious to work with.

If you want to make such a pattern on a cylindrical surface, I see no other way that doing each number/letter in its own sketch. That likely will entail using planes specific to each pattern member, but that's how it is. You have to figure out what minimal number of datums you need to build each instance, group the planes and extrusion of one number, then pattern the group. If your pattern *is* along a helical path, you might be able to employ a helical curve then use trajpar to position each pattern member, etc. An interesting problem, going to require quite a bit of learning to accomplish...

kdirth
21-Topaz I
kdirth21-Topaz I
21-Topaz I
November 17, 2021

You can create an offset surface the thickness of the extrusion.  Then extrude from a plane in the correct orientation and extrude up to the second surface and set the side 2 depth to up to the first surface.  The sketch does not need to be in between the surfaces.

 

If you are trying to go around the cylinder, you could:

  • copy the surface
  • wrap a sketch
  • trim the surface by each number (keeping both sides until the last)
  • thicken each number
There is always more to learn.
tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
November 17, 2021

Review the example in this thread. I think you can use the same approach to generate your desired features. The example is a linear scale but you should be able to use the same approach to place the scale/text on a a circle. 

 

https://community.ptc.com/t5/3D-Part-Assembly-Design/text-repetition/m-p/697310 

L
LukaszMazur16-PearlAnswer
16-Pearl
November 17, 2021

Check my attached model if that's something you want to achieve. I've made it to see if that's possible, so I haven't investigated much why it's considered not regenerated 😉 Model is made in Creo 4.0, BTW.

See sketch relations for the first group in the pattern: there is a relation that sets the number in sketch text to the dimension of sketch point (and converts it to string, as patterning the dimension kept changing the parameter type to real number and it was displayed with many decimal places ;)).

Pattern is used to drive sketch location (sketch text is attached to the datum point on the curve) and incrementing the numbering parameter.

    tbraxton
    22-Sapphire II
    tbraxton22-Sapphire II
    22-Sapphire II
    November 18, 2021

    I suspect that the incomplete regeneration flag is due to your relation being inside the sketch.

    Because the parameter is at Part level, and get assigned different values at the same time, Regenerate state will be unstable

     

    A better and more stable way is to use this approach:

    Create a Datum Point with a placement dimension of value 1

    Create an Analysis Feature that measures the Distance between this point and the placement reference of above dimension
    Ensure to create a Parameter within this feature to store the result

     

    If you refer to the example model I linked to earlier it outlines how to do this and discusses the technique that should regenerate fully.

    https://community.ptc.com/t5/3D-Part-Assembly-Design/text-repetition/m-p/697310 

    L
    LukaszMazur16-Pearl
    16-Pearl
    November 19, 2021
    @tbraxton wrote:

    I suspect that the incomplete regeneration flag is due to your relation being inside the sketch.

    Because the parameter is at Part level, and get assigned different values at the same time, Regenerate state will be unstable

    I suspect you are right 😉 I've found a KB article describing similar approach with the same exact issue of unstable regeneration caused by assigning multiple values to the same parameter.

     

     

    A better and more stable way is to use this approach:

    Create a Datum Point with a placement dimension of value 1

    Create an Analysis Feature that measures the Distance between this point and the placement reference of above dimension
    Ensure to create a Parameter within this feature to store the result

     

    If you refer to the example model I linked to earlier it outlines how to do this and discusses the technique that should regenerate fully.

    https://community.ptc.com/t5/3D-Part-Assembly-Design/text-repetition/m-p/697310 

    Thanks for the suggestion, I'll give it a try. My model was mainly a proof of concept if it's possible to make such geometry. When I'll find the time, I'll see to make it more stable.

     

    M
    MartinHanak24-Ruby III
    24-Ruby III
    November 17, 2021
    @SK_RD8 wrote:

    Hi,

    Can some one help me how do you extrude a scale on a cylindrical part with the numbers from 1 to 10 the easiest way. The only option i have found so far is making a lot of planes and extrude the numbers individual.

     

    I am seeking a smarter way to do it, because i need to do it with many more numbers

     

     

    Hi,

    if all numbers are visible from specific direction then you can use procedure published in https://www.ptc.com/en/support/article/CS25807 document (Offset surface > Expand feature).

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