pattern on PCD

[s_pme20]

hii..
What is the best way to pattern holes as shown..I want parametric dimensions on drawing...I have tried with dimension pattern and added angle dimension in pattern...but it creates pattern with incremental angle...I want all angles with same reference..pls suggest...


View attachment 5331

 

[hemuman]

Try Table pattern!

 

[s_pme20]

hii henuman..
i have tried with table pattern..but it doesnt take angle more than 180 degree...it fails..

 

[s_pme20]

looks like every 1 is in mood of friday..!!!

 

[kdem]

What version are you using? I can get the table pattern to work in WF5.

 

[s_pme20]

hii kdem,
i am using wildfire 4, M150

When i use table pattern, it does not allow me angle more than 180 degree...it consider 180 degree as full circle for me..!!!

 

[faisalmk]

Use pattern around an axis

 

[s_pme20]

Hi faisalmk,
pattern along axis allows only incremental angles...i want each angle to be measured with same reference...

 

[dr_gallup]

I would create the initial feature with an internal angled datum as your orientation (top/bot/left/right) reference. Pro/E has always preferred this. You will be able to put any value in and it will always work.

 

[SRINIVASANIYER1]

Why it does not work beyond 180 deg is due to the reason that the...as thefeature begins to pattern, it take thepositive / negative side of the plane as its starting reference. As you reach 180 deg, you meet with the same reference and it returns.


This was the case in WF1 too. The then recommended procedure was to create a plane, at the desired angle, create a feature at that plane, taking care NOT TO TAKE ANY OTHER PLANE AS REFERENCE, and then group the feature and plane and then perform a group pattern. Try it out


The next best alternative would be to Copy and Paste.

 

[s_pme20]

thanks for help guys...
i have to accept the way it works...though its not fair..!!

 

[kdem]

I got a chance to try this in WF3 and got a mixture of results using the table pattern. Using an extrude feature can cause problems. When I used a centerline in the sketch it caused the holes toend up in the wrong places. Instead try using a construction line from the center of the part to the hole center. For me the pattern generates correctly the only problem that I saw was on the drawing displaying the angle dimensions at 0 (or 360 depending on how the pattern was created) and 180. The angle values displayed from the center of the holes at those locations the othersdisplayed correctly. When using an embedded datum the pattern generated correctly but only the pattern leader angle dimension displayed. Pulling the datum out of the extrude feature,grouping the items, and patterning the group allowed the angle dimensions to show correctly on the drawing. Another thing that worked is creating a hole feature and table patterning. I'd say it also depends on how you are modeling as to the results you'll get.

 

[s_pme20]

yes kdem,
you r right...extrude with centreline creates problem in identifying correct angle direction..
I think best way is to create radial hole (with one angle and one radial dim.)..and then using table pattern for angle...

thanks..

 

[srieger]

You can get this by creating dimensions in the drawing. These dimensions are still parametric. They are simply driven dimensions vs. driving.