DRAWING: add fastener pattern without having a hole feature

[pvn]

Hey guys,

please help. I need to have a drawing with a fastener pattern call out. Something like this.

We do not have time to detail holes in parts and fasteners though. I only have a sketch with the holes locations in the part (to make sure we are not having any interferances and plenty of edge margin).

Is there a way to just show the crosses in the locations driven from the sketch?

Thank you so much for your help.

[dschenken]

Create a sketched curve feature and you can use that. The sketch may include a datum axis point for convenience.

[pvn]

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@dschenken wrote:

Create a sketched curve feature and you can use that. The sketch may include a datum axis point for convenience.

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Do you mean Extrude as a surface?

I already have a hole sketched, but I can't figure out how to add hole centerline on the drawing.

[RoyCrerar]

I mean add to the model the Hole. There is a hole command you might want to read up on that as it can do a lot of things for you. CSK/Cbore tapped etc and give you nice std notation. it also can show up in hole tables if you fancy driving that too.

Once the hole is in you get an axis for free which can be shown in the drawing as you would expect. use the show annotations in Annotations tab.

I would be surprised if you ever need to sketch a hole that cannot be generated by the Hole command, it just takes a little familiarisation. 

[pvn]

Thank you. There's a reason I don't need a hole feature in the model. Otherwise I wouldn't be asking for help here. This hole pattern is for manufacturing reference. The holes will be drilled on install. I do not and can't control their location at this point.

[TomD.inPDX]

I might suggest using datum point sets in the model (quick to hide).  They can have intelligent names to some extent.  In the drawing, you would create point features [sketch] ...linked to the model's datum points.  Once you have the drawing points, you can hide the datum points.  This is just one way to manage both model features and drawing visible features on an individual basis.  Either point set, Model or Drafting Sketch, may also be useful for pinning down annotations on the drawing... but that needs to be tested for ease-of-use. 

You can add more intelligence in the model if this is a way of doing business.  It is a simple ROI calculation.  One thing PTC does well is allow for programming all this into the model, somehow.  You would simply "show" the annotation on your drawing and will be orientation sensitive.  It is all about codifying a defined process.  You'd be amazed at what's in the Creo toolshed for all of us to use.

[pvn]

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@TomD.inPDX wrote:

I might suggest using datum point sets in the model (quick to hide).  They can have intelligent names to some extent.  In the drawing, you would create point features [sketch] ...linked to the model's datum points.  Once you have the drawing points, you can hide the datum points.  This is just one way to manage both model features and drawing visible features on an individual basis.  Either point set, Model or Drafting Sketch, may also be useful for pinning down annotations on the drawing... but that needs to be tested for ease-of-use. 

You can add more intelligence in the model if this is a way of doing business.  It is a simple ROI calculation.  One thing PTC does well is allow for programming all this into the model, somehow.  You would simply "show" the annotation on your drawing and will be orientation sensitive.  It is all about codifying a defined process.  You'd be amazed at what's in the Creo toolshed for all of us to use.

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Thank you. That's on thing I was thinking about. Just do points.

I would really love to explore more inteligent ways of working with Creo. I wish it was a bit more new user friendly 🙂 Is there any articles you know that can be of help?

[RoyCrerar]

see attached

[wfalco]

You can create axes for holes and show in drawing (if used)? But I would think you'd want the "whole hole" to show tangents to your max border? I assum the holes may be other than simply thru diameters? This is why you want simple?

[pvn]

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@wfalco wrote:

You can create axes for holes and show in drawing (if used)? But I would think you'd want the "whole hole" to show tangents to your max border? I assum the holes may be other than simply thru diameters? This is why you want simple?

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I only need to show the centerline of each hole to represent rough location. In this case manufacturing would have a better view on how to locate the fasteners. On top of that we are pushed by time and absense of the standard parts library or any experienced Creo users 🙂

I added an axises for a few holes but can't seem to figure out how to show them and how to attach a centerline of the hole.

[wfalco · Accepted solution]

In drawing: annotate(top tab)>show model annotations(left lower tab)>show model datums (right top tab)>type(pulldown):axis>select part

Not sure what you mean by attaching cl to hole?

[pvn]

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@wfalco wrote:

In drawing: annotate(top tab)>show model annotations(left lower tab)>show model datums (right top tab)>type(pulldown):axis>select part

Not sure what you mean by attaching cl to hole?

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That works! Thank you so much. I couldn't wrap my brain around as to how select the features I want to show by using Show Model Annotations. And it's just clicking on the part 🙂 

[wfalco]

UR welcome. It is not intuitive.

[RoyCrerar]

Hi,  It probably took longer to do the sketch than pattern a few holes. Once patterned the first fastener is added then you parttern by reference and you have all in position correctly. If you are smart enough when you define the fastener you can define the assembly constraints so when the first one was assembled you wouldn't need to even select the fastener constraints.

If you know what you are doing you can add hundreds of fasteners quickly and easily. You also get the benefit of having accurate automated BOM's that you can't get from a sketched set of centres.