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J
jchance11-Garnet
11-Garnet
May 20, 2026
Question

Reference Patterning Sketched Hole Patterns

  • May 20, 2026
  • 7 replies
  • 84 views

several ways to go about this and i’m struggling to find the ideal method

 

  1. Create external sketch
    1. place hole on sketch and choose end points/midpoints/etc
    2. Place a fastener in hole (standard coincident/mate)
    3. Reference pattern doesn’t work
  2. Create sketch INSIDE of the hole tool
    1. sketch my shape
    2. place fastener
    3. reference pattern doesn’t work
  3. Create an external sketch
    1. sketch using datum points
    2. Place hole on point
    3. pattern by on point
    4. Place fastener in hole and pattern by On Point
    5. Choose the previous points to pattern by
      1. This works!
  4. Create a sketch inside of hole tool
    1. sketch with lines and place datum points on end points
    2. holes are created
    3. reference pattern and point pattern doesn’t work

Am i missing something here?


if i want to reference fasteners in the holes i placed while using a sketched pattern i need to:

  • create an external sketch
  • place datum points on sketch end points(or mid points or whatever)
  • pattern by on point(which is my selecting a point pattern​​​​​​

7 replies

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
May 20, 2026

It’s difficult to give you advice without some sort of context of the application. Simple square hole patterns are easy and radial hole patterns are easy but maybe you are dealing with something unique that simple doesn’t apply.

tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
May 20, 2026

As ​@StephenW has indicated there is not enough information to reply specifically to your inquiry requesting an ideal approach to a problem. There is likely not a single best way to deal with a given scenario when accounting for design intent, workflow, team interaction, and deliverable work products out of Creo.

 Clearly outline the design intent you need to control and how you would like to control it along with what version of the Creo you are working with. It seems that you are wanting to leverage patterns in a part and extend the pattern reference to assembly mode to facilitate the placement of fasteners. Reply with a detailed problem statement and you will get some good feedback on how to deal with the issue.

    J
    jchance11-GarnetAuthor
    11-Garnet
    May 20, 2026

     External Sketch of the holes i want to place is Sketch 3.  i had to place datum points at the corners where i wanted the holes.

    Fastener placed in hole 

    pattern by reference isn’t an option. i can only pattern by On Point.  Which means i have to place datum points on the corners of the sketched hole pattern(external sketch 3). This also means i can’t use “sketched” inside of the hole tool either to place items at the assembly level

     

    S
    23-Emerald III
    StephenW23-Emerald III
    23-Emerald III
    May 20, 2026

    Always depends on the specific design requirements, but something like this, I would simply place the first hole to the “primary” corner and then used a dimensional pattern to get the other holes.  The right answer is the one you are most comfortable with and feel provides the dimensional controls you need along with, in this case, the ability to use a reference pattern. Sketch patterns are “special” and don’t always provide all the pattern functionality (my opinion)

     

    J
    jchance11-GarnetAuthor
    11-Garnet
    May 20, 2026

    I think both of you have illustrated that I'm not doing anything wrong and that using a sketch to drive a pattern doesn't actually let you use reference pattern at the assembly level.  

    the workaround is what I'm already doing, which is to place points on the sketched pattern I want to use.  Unfortunately you can't utilize points if you make the sketch INSIDE of the hole tool. So while it's nice that Creo added functionality to the hole tool, it's relatively useless for adding fasteners to it.

     

     

    I'm well aware of directional, axis, and dimension patterns. I understand that they can allow reference patterns at the .asm level.  Sometimes it's easier to have a more robust design that can be easily edited when making my patterns based off sketches instead of dimensions or directions.  If I want to have the holes always be spaced off certain cutouts and those cutouts are open to dimensional changes then a sketched pattern is the easier way to go.  Even moreso if utilizing a family table instance.

     

    Thanks for the help and clarification.  This would be a nice upgrade in Creo if they allowed reference patterns based of sketch end points and not just datum points

    tbraxton
    22-Sapphire II
    tbraxton22-Sapphire II
    22-Sapphire II
    May 20, 2026

    Sketch patterns (within assembly components) can be referenced at the assembly level. Two examples below, the second of which is a sketched hole driven design intent. Here is a sketched pattern in the plate that is used in the assembly for reference pattern to place the fasteners. See the reference viewer for the dependencies. There are multiple ways in Creo to leverage the pattern as you desire.

    Check out the green array of fasteners below which I believe is created in the manner that you desire, please confirm. Note that for the green pattern no datum points are explicitly defined in the sketch embedded in the hole feature of the plate.

     

    Sketch pattern of points used to place holes in the part and fasteners in the assembly by reference
    Sketch containing points used to define hole locations

    Here is an implementation of a sketch made in the hole feature of the plate that is leveraged in the assembly to place fasteners by reference.

     

    Reference pattern placement of the green fasteners at the corners of a sketched rectangle in the hole feature of the plate
    Embedded sketch in hole feature to create rectangular array of holes used in assembly for reference pattern placement of fasteners
    Take note of the hole placement options for the sketched hole functionality

     

    tbraxton
    22-Sapphire II
    tbraxton22-Sapphire II
    22-Sapphire II
    May 20, 2026

    This is one method to deal with the pattern such that you only create one pattern in the part and are able to leverage that for the holes in the part model and the fasteners in the assembly containing the plate with the holes. It is not the only way to address this re-use of the pattern definition in the part.

    In part mode (the plate with the clearance holes), create a point pattern to define the hole center locations. The exact details will vary according to the geometry and hole locations. Add a hole to the plate using the placement surface (top of plate) and the pattern leader datum point. Pattern the hole using the reference pattern option.

    Point placed using pattern along a datum curve evenly spaced
    Pattern the hole using the reference pattern option
    In the assembly place the first fastener using the hole at point pattern leader and pattern the fastener by reference

     

    Michael
    16-Pearl
    Michael16-Pearl
    16-Pearl
    May 21, 2026

    Create a hole and use sketch as dimension scheme. Put datum points in the sketch where you want holes. Finish defining your clearance holes. This actually creates a pattern. Now in assembly mode, use intelligent fastener and choose any of the clearance holes surface as location. IFX will ask you if you want to pattern the fastener. Choose yes. 

    Michael Bourque
    J
    jchance11-GarnetAuthor
    11-Garnet
    May 21, 2026

    We don't use IFX.  It's not compatible with our BOMs

    Michael_Bourque
    Michael_Bourque10-Marble
    10-Marble
    May 21, 2026

    You don’t need to use IFX. Even if you use a regular bolt part, placing the bolt in one of the holes will allow a reference pattern:

    Create a hole and set Sketch as the dimension scheme. In the sketch, place datum points wherever you want the holes to appear. Finish defining the clearance holes; Creo creates them as a pattern.

    Then, in Assembly mode, assemble one bolt and select the hole surface as the placement reference. After the bolt is placed, select the bolt and use Pattern > Reference to pattern it to the remaining holes.


     

     

    Michael Bourque
    tbraxton
    22-Sapphire II
    tbraxton22-Sapphire II
    22-Sapphire II
    May 21, 2026

    Watch this video showing the use of an external sketch used to define hole creation and reference pattern placement of fasteners using the sketched hole feature. This is taken from Creo 10 session.

     

      Michael_Bourque
      Michael_Bourque10-Marble
      10-Marble
      May 21, 2026

      This is the exact workflow I just suggested. Excellent!

      Michael Bourque
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