Hole Pattern Dimensions in Drawing
Hole Pattern Dimensions in Drawing
(OP)
When you create a pattern in a part, the pattern feature only gives you the option to define the spacing distance between features. Then in the drawing, the model dimension that shows up is the spacing dimension. I would like to have each hole dimensioned from the end of the part to minimize tolerance stack-up.
Is there a way to change the model dimension(s) of the pattern so that each hole is dimensioned from the same location on the part? I prefer to show model dimensions in my drawings rather than creating them, but it seems that I don't have that option here.
I think I remember being able to change this in Pro/E, but it has been a while since I've used Pro/E, so I'm not sure.
Is there a way to change the model dimension(s) of the pattern so that each hole is dimensioned from the same location on the part? I prefer to show model dimensions in my drawings rather than creating them, but it seems that I don't have that option here.
I think I remember being able to change this in Pro/E, but it has been a while since I've used Pro/E, so I'm not sure.






RE: Hole Pattern Dimensions in Drawing
RE: Hole Pattern Dimensions in Drawing
RE: Hole Pattern Dimensions in Drawing
I assume you mean creating all of the instances in one feature instead of patterning? The only problem with that is it makes it tough to add fasteners to the assembly when you can't follow the pattern.
RE: Hole Pattern Dimensions in Drawing
YOU CAN MAKE A SKETCH OF POINTS YOU WANT IN THE PATTERN AND DO A SKETCH DRIVEN PATTERN.
This will allow you to use Sketch pattern to get a good 2 directional pattern. and add reference dims.
This will create a pattern similar to pro/e's table pattern.
If you create a sketch pattern you can delete the relation and use fully define sketch with ordinate dims to get each dimension called out as a driving dim or keep the pattern relation and use the Ordinate as ref dims.
What CBL is suggesting is to do linear pattern using the offset dimensions from the hole placement sketch to do the pattern which as a Pro/E user you know used to be a requirement for patterns before they Direction Pattern was created. That may give you the dimensions in the pattern instances but I know that the Sketch Driven does. I'll try to do and post an example in 2009 and 2010 formats.
Michael
RE: Hole Pattern Dimensions in Drawing
RE: Hole Pattern Dimensions in Drawing
Do you absolutely have to display model dimensions on your drawing?
Apply reference dimensions. You can set these up any way you darn well please, while you model your features any way you darn well please.
RE: Hole Pattern Dimensions in Drawing
Creating dimensions in a model and then recreating those dimensions (or creating other dimensions) in the drawing seems redundant. Not to mention creating dimensions in the drawing allows for accidental over dimensioning and other mistakes.
I see a lot of older drawings here that have dimensions created in the drawing and they have somehow become detached from the features they were dimensioning. These dimensions are usually grey and have an incorrect value. That wouldn't have happened, had the person shown the model dimensions.
RE: Hole Pattern Dimensions in Drawing
Eric
RE: Hole Pattern Dimensions in Drawing
If you can indeed pattern fasteners to the hole wizard set of holes (as mentioned by CBL), then I will definitely just create them that way. I had previously been creating the holes using the hole wizard, anyways, and inserting the fasteners one by one. I'll have to try to patterning the fasteners the next time it comes up.
RE: Hole Pattern Dimensions in Drawing
NOTE: When creating the pattern, any hole can be selected as the 'virtual' seed hole, but I prefer to use the 'real' one.
RE: Hole Pattern Dimensions in Drawing
Wish I had this information months ago. I've been wasting my time inserting fasteners one at a time.
RE: Hole Pattern Dimensions in Drawing
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