patterns in Pro-Engineer 1

[AKB]

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.

 

[npsingh]

Dear Mr.,
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

 

[ng]

dear friend,
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

http://www.hitechesoft.com

 

[Recneps]

Two major common mistakes made when patterning:

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

 

[tsankar]

Hi,
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

 

[Recneps]

Unfortunately, the Copy>Translate THEN use Pattern command method produces two distinct features unless they are manually grouped.

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

 

[tsankar]

Yes, I agree with Recneps.Incorporating the dimensions you would use for the pattern as a part of the original feature sketch is definitely better.

TS

 

[debanjan]

Make an 'on the fly datum' with an angular dimension (even if the angle value is 0) wrt to some other Datum plane. Then to pattern select this angular dimension as the incremental dimension. I guess this'll solve your problem.
Debanjan
db@hitechesoft.com

 

[ng]

i am working in software division of a gear mfg. company.We are using Swept Blend Option to create Helical Tooth. Using this technique we can't directly pattern the first tooth, because when you create a feature using Swept Blend, pro/e never ask to choose a plane for selecting Datum Curve/s.
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

http://www.hitechesoft.com