I am trying to use the fill pattern feature in Creo Parametric 8.0. I am simply trying to create some small 3.0mm holes for vents for an electrical cover box. I have performed the following steps:
- I have created a rectangular sketch (used for the Fill Region/Grid)
- created a hole using the extrude feature that is positioned on the same surface within the bounding box
- I have tried constraining to the center of rectangular sketch in "bullet point 1", but this doesn't make any difference in my end result
- I get a preview showing the features that will get patterned
- I click "OK" and the features are created very far out of the bounding box I created in "bullet point 1"
- I have tried creating the sketch within the pattern feature as well, with no luck
Every time I try this, using other shapes (hexagon's, squares, etc) as the feature shape, I never get the pattern actually made within the boundary box that Creo Parametric allows you to define.
Any idea what is happening here, or is this a bug others have seen as well???
Change you pattern leader definition/dimensioning scheme. You must account for the offsets of the fill pattern in relation to the filled sketch region. This is one way to deal with this easily, by sketching a rectangle that anchors the pattern leader in the upper left corner which will work nicely for a rectangular array of fill which is what you need. Note the hole is placed at the upper left corner of the fill sketch and the offset to the interior of the fill pattern is 0. You can also get this by using the offsets in the fill pattern definition (your approach using the sketch for fill with an offset to the interior).
Hey @tbraxton thanks for the quick reply! That does make sense that the positioning should be in the corner of the rectangle since it is a rectangular pattern.
I do not quite understand what you are trying to say in the last sentence of your reply "You can also get this by using the offsets in the fill pattern definition (your approach using the sketch for fill with an offset to the interior)." Can you elaborate please? Are you saying that I can't use the offset from boundary surface if I pattern this how you suggested in your pictures?
Do you suggest that these fill pattern boundary sketches be made within the Pattern Feature? Or creating the sketch before the pattern feature, and linking the leading circle extrude to a vertex on the boundary sketch?
Following your suggestions above, I am still getting this weird offset:
No idea why it is so different than yours.
I would need access to your model to diagnose it expediently. If you can post the model, then I will have a look at it. I think the behavior you are getting is based on how the pattern leader is constrained/dimensioned (to be sure I need to query the model).
I did the test model in Creo 9 so you would not be able to open it. I would also use a hole feature and not an extruded cut (both should work in theory) for the pattern leader. Here is the model tree and the hole I used to create the centered pattern. Note the dimensioning scheme used to locate it on the corner of the fill sketch. It should make no difference if one uses an external or internal sketch for a fill pattern. I would typically use an external sketch created prior to the fill pattern being defined but that is preference. Try to mimic the scheme used for the pattern leader shown below and see if it changes pattern in your model.
Here is a Creo 7 model that follows (I think) your design intent and uses a hole centered in the fill box as the pattern leader. As with the above example the pattern options and dimensions may result in undesirable results.
