patterns in Pro-Engineer
patterns in Pro-Engineer
(OP)
I am trying to create a gear. I have created one tooth and would like to pattern the tooth to complete the gear. I try using pattern and do not understand why it fails. I would like to know in detail how to pattern the tooth.





RE: patterns in Pro-Engineer
You have not mentioned the steps you followed but I expect that you have created the feature on an internal datum plane passing through central axis and angle with one DTM Plane. Now these steps should be followed:
Pattern ---->(select feature)-----------> Identical and then enter the angular value for gear spacing and number.
I don't think this can create any problem although this is not the best method to create Gear.
Please write the steps you followed are contact me for better method (In my knowledge)
Narendra
N P Singh
RE: patterns in Pro-Engineer
first you make a copy of the first tooth using copy rotate about central axis and angle is (=360/teeth).Then pattern the second teeth using varying or general option & dim 360/teeth and no of paattern is (=teeth-1).
nikhil gothankar
ng@hitechesoft.com
www.hitechesoft.com
RE: patterns in Pro-Engineer
1. The initial feature MUST have a dimension to another feature/datum, etc...patterning function won't use a dimension that relates to the same feature. My most common fix for this is to make a datum 'on the fly' that goes THROUGH the central axis and at an ANGLE to a perpendicular datum when creating the first feature. This gives a perfectly usable dimension for patterning (angular dimension).
2. The two major types of patterns are also a source of confusion. Depending on the type of pattern you are creating, you will use either IDENTICAL or GENERAL. General takes more time to regenerate, but allows the flexibility to have the patterned features overlap while still creating a 'single' solid. Identical is for the more simpler patterns...you should be able to use Identical for the gear teeth.
Recneps
RE: patterns in Pro-Engineer
You can make a copy of the initial feature using COPY-TRANSLATE-ROTATE (the rotation angle being the angle between 2 tooth) and then use the copied feature for generating the pattern.
(Of course, give the correct number for the number of pattern instances)
TS
RE: patterns in Pro-Engineer
Utilizing design intent and incorporating necessary dimensions into the original feature sketch, then patterning creates a nice, clean solution. When your part is a complicated one, every little thing you can do to make your design cleaner helps.
Recneps
RE: patterns in Pro-Engineer
TS
RE: patterns in Pro-Engineer
Debanjan
db@hitechesoft.com
RE: patterns in Pro-Engineer
So first we create a rotate copy of the first tooth, then we use pattern option to create full gear.
nikhil gothankar
ng@hitechesoft.com
www.hitechesoft.com