Extrude numbers from 1 - 10 helical on a surface

[SK_RD8]

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

[KenFarley]

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]

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

[tbraxton]

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 

[LukaszMazur · Accepted solution]

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.

[KenFarley]

That is exactly as I pictured it in my head. Nice.

[SK_RD8]

 Thanks

[LukaszMazur]

Thanks 🙂

[SK_RD8]

That was what i where looking for, thanks. 

Where/how do i see the relation for the Numbering?

Thanks

[LukaszMazur]

Go into Pattern 1 of LOCAL_GROUP > Group LOCAL_GROUP and Edit Definition of Sketch 1. While in sketcher change tab to the Tools tab and click Relations from the Model Intent group. You'll find a relation there:

number = itos(floor(sd3))

sd3 is a dimension of sketcher construction point (sketcher construction point is not visible outside the sketch, so it can be used to change dimension value tied to the parameter without actually modifying any geometry; it's a workaround for lack of loops in patterns/relations).

[tbraxton]

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 

[LukaszMazur]

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@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

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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 

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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.

[MartinHanak]

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@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

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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).