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Point Pattern - How to access the number (count) of Pattern Members

kpritchard
4-Participant

Point Pattern - How to access the number (count) of Pattern Members

Hi All,

Any ideas how to get the number of Pattern Members when using a Point Pattern? I'm not looking to drive the number of Points in the Sketch with this, it's display only. Use case is an irregular pattern of holes, and everything works fine except I don't have a way to add the number of holes to the hole callout. On a Dimension (and Table Pattern I think) this shows up as a parameter that can be added.

Thanks in Advance

13 REPLIES 13

I am also searching the same not only for point also for fill pattern. I guess you may need to add an idea.

This sounds like an extension to this idea:

http://communities.ptc.com/ideas/3639

If everybody votes it up, maybe PTC will implement it in Creo Parametric 14.6, or perhaps even sooner...

Dale_Rosema
22-Sapphire I
(To:JWayman)

Over 3 years later, is this still not possible?  I'm driving hole features by a point pattern in Creo 2 and Creo knows the number of holes because it adds it to the hole note, but I cannot reuse it elsewhere. 

In the hole note it's &PATTERN_NO, but that doesn't work anywhere else.  I tried &PATTERN_NO:fid_3047 where 3047 was the feature ID of the pattern and that failed as well.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

[Edit] I misunderstood your question. Sorry about that. I don't know the answer to your question. Hopefully you found a way.

 

[Original Respond]

Fortunately there is a way, although not very intuitive (you all know how user friendly Creo is). Choosing your pattern feature, right click and click Edit (NOT Edit Definition), the dimension will be displayed without going into the Pattern function. Hover your mouse pointer above the number of pattern dimension, and if should display the dimension pxxx:Fxxx(PATTERN), then you can use that pxxx dimension, or you can click Switch Dimensions and it'll show the variable too.

3 years late, but hopefully other people will find this helpful.

 

Good luck.

the described method may work for a circular pattern like in the below linked video, but in my case i have holes located by 4 points at the corners of a construction-line rectangle. when i click & select edit dimensions, the dimensions of my construction-line rectangle are shown, not the # of instances of holes.

 

https://www.youtube.com/watch?v=HpzO3HqrbO4

Sonther
4-Participant
(To:wnicsir)

Hey, this works fine as long as you actually use all of the holes in the pattern. If you "click" away some of the holes, the pattern name id still calls out all of the holes (even the ones not active).

I've come here looking for a solution to the same problem.

What's the point in Creo offering a function to de-select specific holes in an array to create irregular patterns but then have the notes feature for the array totally ignore the exclusions. Seems absurd that for such arrays, I have to manually type in the hole quantity, essentially overriding the link with the model.


I find it hard to believe this was an intentional feature by PTC & come to the conclusion that it was simply not thought of as being a problem.

I'm using Creo 4 but upgrading to 8 sometime soon. It would be nice to think some of the awful inadequacies of Creo drawing will be fixed but I don't hold out much hope sadly 😞

Chris3
19-Tanzanite
(To:PT_8224451)

If you are looking for a solution for hole notes this has been delivered in Creo 8:

https://support.ptc.com/help/creo/creo_pma/r8.0/usascii/index.html#page/whats_new_pma/core-new_note_... 

sacquarone
19-Tanzanite
(To:Chris3)

Hello @PT_8224451 

 

Confirming what @Chris3 said earlier (Thanks Chris!!). This Creo 8.0 enhacement applies for patterns of standard holes (including point pattern) and is: 

  • Documented also in article 355440
  • Illustrated for you in little movie below

 

Regards,

 

Serge

 

pausob
17-Peridot
(To:sacquarone)

??? it has worked like this for a long time for "standard" holes.  PATTERN_NO token in hole notes always displayed the actual instance count.  As far as I can tell, the Creo 8 enhancement is that the tokens now will become blank in the cases where the pattern count is only 1 - avoiding the clumsy 1X hole callout...

 

However, I have to just wonder how the work to deliver this enhancement was prioritized over the requests to have the PATTERN_NO or INSTANCE_COUNT as a feature parameter in any pattern so that it's available for use in notes and calculations. 

 

so, go and vote on this idea: Number of instances in a point pattern.

 

sacquarone
19-Tanzanite
(To:pausob)

Hello @pausob 

 

You're right. My example was not really relevant to show how Notes of hole pattern are improved in Creo Parametric 8.0 (except it was using &HOLE_INSTANCE_COUNT new hole token, instead of former &PATTERN_NO in my example).

=> For others who may be interested by an exhaustive overview of what is excatly enhanced in this version related to Hole Pattern & related new tokens introduced, please refer to this movie here.

=>  For the request to get this effective for any pattern (and not only hole patterns), I confirm it's not part of Creo 8.0 capabilities, so that only suggestion I can share is indeed to vote on this idea: Number of instances in a point pattern.  (Consider however it is currently reported in the direction of "point patterns", and not really "any pattern")

 

Regards,

 

Serge

There is a way, if you use a secondary tool. You can write a script to analyze the program code and count the holes there. I use the freeware CreoSON for it, and afterwards add it to the dimension text. But it is not simple to achieve and will not automatically update when you change the pattern.

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