Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

little help on patterns

vikas02121

New member
hi,

i m a pro/e novice and i m mailing for the first time.

I have a problem in making a pattern.

Actually , i m trying to make a pattern(angular) of the cylinder on the top of a circular disc but till now i m unsuccessful.

but i created a pattern of hole on the disc successfully.

plz help me out of it



thanx

vikas
 

Jake

New member
To create a pattern of a sketched feature in an angular direction you must have created the feature with an angular dimension. Create the cylinder as before except when asked for a horizontal or vertical reference plane for sketching choose Make Datum from the menu and choost through and pick the axis down the cewnter of the disc and then angle and pick a plane to be at an angle to. awhen you now pattern it, pick the angle dimension and continue from there.
 

adicar01

New member
Reference plane for sketching one dtm or plane surface, BUT for orientation (sketch-second plane) by ex. top, choose make a plane through cilinder axis, and angular for one plane (you can put angular dimension = 0, or put any, and after that you can modify



[email protected]
 

satish

New member
Dear vikas 02121 what Mr. adicr01 had sujested for the pattern is correct. Follow the same technique. If you cant follow the technique send the prt file to us. let us work on it.
 

xcad

New member
hello my friend. You know pattern in Pro/E is something very interesting. You can do thinks that even you haven't imagine. My advide is to search in search machines with the correct key words every time and find what you want. By this way you will find excellent thinks about Pro/E, and even about the pattern command.

Enjoy the feeling discovering something.... different every time, and remember there is nothing somebody can't do in Pro/E.

[email protected]
 

kax

New member
I think that you dont have to make datum pattern for an angle pattern.

1. Just create the feature you want on any plane.

2. Then copy - move - rotate the feature you just created and select a curve - edge - axis on which you will rotate.

3. After this you have now two (2) features.

4. Delete the first feature

5. Create a pattern of the new feature and you will use of course the angular dimension which appears.
 

Falkirk21

New member
I am having the same problem.



Is there a way to make an anglular dimension to the cylinder when you are creating the original drawing without making aditional datums or copy/move/rotating the cylinder?



Any help on this would be very helpfull.
 

kvision

Moderator
to create an angular pattern that correctly shows the dimensions for the feature when picked and allows you to do ref pattern on the whole pattern requires a Make Datum. Why?

If you create the plane ahead of time the dimension will NOT appear when patterning the feature. You will be forced topattern the plane and then pattern the feature. If you use the copy move technique you will NOT be able to use ref pattern on all the features. For example if you add a bolt to a hole in an assembly you can't ref pattern ALL of them at once. You will be forced to add the bolt at least twice.

For sketched features you USUALLY choose an existing sketching plane and then for the SECOND plane which is the horizontal or vertical refernce plane you need to create a Make Datum, thru the central axis and at an angle to another plane. The angle can be 0. finish the feature normally. When you pattern that feature the angle associated with the Make Datum will appear. The Make Datum is an internal datum and does NOT appear as a feature in the model tree.
 

kvision

Moderator
to create an angular pattern that correctly shows the dimensions for the feature when picked and allows you to do ref pattern on the whole pattern requires a Make Datum. Why?

If you create the plane ahead of time the dimension will NOT appear when patterning the feature. You will be forced topattern the plane and then pattern the feature. If you use the copy move technique you will NOT be able to use ref pattern on all the features. For example if you add a bolt to a hole in an assembly you can't ref pattern ALL of them at once. You will be forced to add the bolt at least twice.

For sketched features you USUALLY choose an existing sketching plane and then for the SECOND plane which is the horizontal or vertical refernce plane you need to create a Make Datum, thru the central axis and at an angle to another plane. The angle can be 0. finish the feature normally. When you pattern that feature the angle associated with the Make Datum will appear. The Make Datum is an internal datum and does NOT appear as a feature in the model tree.

If you copy and then delete the lead feature you are increasing the cpu time for large patterns. If you are using a small pattern then this should be a good shortcut.
 

Sponsor

Top