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

[kpritchard]

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

[jsarkar]

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

[JWayman]

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]

Corrected link:

Create an Automatic Parameter for total pattern members

[dgschaefer]

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.

[wnicsir]

[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.

[ryanmoore0001]

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]

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).

[PT_ChainsGuru]

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]

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_tokens_patterned_holes.html 

[sacquarone]

Hello @PT_ChainsGuru 

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]

??? 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]

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

[PT_ChainsGuru]

2 years later I still can't get the correct hole array count to report correctly.

To clarify, I don't use points & simply use the hole feature using a central axis for the PCD & plane as angular constraints.

These are plain drilled holes with countersink either side so there are no hole notes as you would get in threaded holes.

As a result, the HOLE_INSTANCE_COUNT or PATTERN_NO have no effect on the actual hole count. The only hole count & can get to report is the P78 as featured which reports the full 16 hole array.

In the first graphic I've shown the actual 16 hole array illustrating the 3 I want to keep.

In the second graphic I've shown the text I typically append to the first hole in the array to report the hole count, diameter & PCD.
I've added the top line to illustrate how the HOLE_INSTANCE_COUNT doesn't work in this instance.

If I'm doing something wrong here I'm more than happy to be corrected

[pausob]

Not sure why HOLE_INSTANCE_COUNT doesn't work...  Maybe because these parameters are only available in "table driven" holes, and not plain ones as you describe?

Anyway, not sure which version it appeared, but for sure in Creo 10 you can call out in your notes / relations a feature-level parameter called PTC_ACTUAL_PAT_MEMBERS:

This parameter exists in pattern features and also the new multi-point sketch hole features.

(in this example, this would be called out in a note using syntax &PTC_ACTUAL_PAT_MEMBER:FID_1343680)

(in this example, this would be called out in a note using syntax &PTC_ACTUAL_PAT_MEMBER:FID_1343539)

yes, it is tedious to have to make a custom note for each hole pattern, but it enables making correctly updating parametric notes.

[PT_ChainsGuru]

Thanks for the detailed response. We're upgrading to 10 shortly so I look forward to finally having a working solution for this.

I've had a look at a document detailing the difference between 8 & 10 & can see a number of improved features of interest.

There are so many incredibly annoying "features" in Creo drawings that are absurd that any improvements usually result in a loud cheer in the office.

I don't know whether this is true but I was told by someone that has worked closely with PTC for a very long time & said that the developers deliberately haven't spent a lot of time developing the drawing side of things.

The reasoning was that they believed everyone machines to as 3D model so a decent drawing wasn't needed.

I've been working in design for over 40 years now having started on the board & only in the last few years have people started using CAM models.

Not every company has the luxury of modern CNC equipment & many subcon folks are still using manual machines.

[ptc-5132323]

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.