Rotational pattern

[urfriend]

No Dr_gallup even for the simpler feature i couldn't do it successfully ! I want all the 3 instances equispaced at 120 degrees.


I've tried to re-create it from the begining many times!


Dear rcamp i did not refuse to use the datum curve option.


[there also i got a problem. that when i pressed extrude, then create a datum curve, then TOP plane as the sketching plane, referenced to the central axis, & drew a datum curve. But when I pressed CONTINUE WITH THE CURRENT SECTION button, I got a WARNING ( See pic below) After continuing , the feature was not created (regeneration failed ) ]


View attachment 1842


A Request: your friend , your colleague, your company, your workstation, somewhere you may see WF1. Please getit done this pattern in WF1 & upload it. I'm dying to see this happened !! ( otherwise slowly i would loose my faith that this can be done without problem)


1 more question: how to dimension 2 points lying on an inclined line? ( in the figure below dimension between axis & center point of the circle ) (NOT X & Y values but polar dimensions length & angle)


View attachment 1843

 

[AHA-D]

The "magic" of construction lines will help you !


In the above example draw a line, give it an angle dimension and a length dimension. Click on the line, then RMB and choose for "toggle construction". The line is now part of the sketch but won't be used as feature geometry. Now connect the centerpoint of the circle to the end of the line.


The result is a circular cutout that you can position at any angle and any distance from the center.


Alex


attached picture showing similar construction


View attachment 1844
Edited by: AHA-D

 

[dr_gallup]

Here is a part made in R20, that is the only pre-WF2 build I have loaded. It will be a little different because the rotational datum is built "on the fly" and is not visible or in the model tree. But you will be able to open the part in WF1.

2006-02-17_121235_rev_pat.prt.zip

 

[urfriend]

Hurray........!!!!

Thanks, thanks, thanks,......thanks a lot!!! (Now this is the joy of pure happiness)


I just can't tell you how much i'm happy after seeing it happened !!


Would you like to know the blunder i was doing??
( I must tell you considering your outright help !! )


The blunder I found: ( Which I could see, only by investigating the model posted by you - thank you very much, how nice of you! )


After making the datum on the fly & resuming the extrusion feature creation,
we are asked to select sketching plane.


I used to select the TOP (default) plane as the sketching plane & The RIGHT plane on the RIGHT side for its orientation. (Which was the unforgivable mistake.)
I should have selected the datum created on the fly (Datum 1) on the top side for oritntation.


When I was asked to select the references for the sketcher placement, I used to ERASE the default planes TOP & RIGHT from the references window and reselect the central axis & the datum plane as the references.



(Which might be conflicting to Pro/E because the references BEFORE entering into the sketcher & INSIDE the sketcher environment were different)


In your 2nd reply you had told me to select central axis & the datum on the fly as the sketcher references. Even though I was giving those references the method was incorrect!!
( Specifying the references for oritntation,has always been a problem with me. Can you help me better in this particular area?)


Also one more inexcusable thing was, NOT adding the "OUTER SURFACE" to the references window. Because of which my pattern was not revolving 360 degrees.


All the things I could have not found without your precious help!!


Thanks once again, to all you guys & especially dr_gallup for literally pulling me out of the problem !!

View attachment 1846


Watch the most satisfying command line !!






Don't Kill me Please.......!!

One more question i had asked "about giving aligned dimension between 2 distant points on an inclined line".
Again a WISE alternative has been suggested !!! (by AHA-D)


"In Pro/E has everything to be created the OTHER WAY ROUND?" ( & Not by the simpler straightforward method !!)
(Even in 2D AutoCAD also, we can give this kind of aligned dimension EASILY ) then why not in so advanced Pro/E?


I'm sure you must have some answer!!

 

[sip]

Yes. ufriend.


The dimension you want to make between 2 points on an inclined center line is very simple indeed.


Pick dim, pick th 2 points, and middel-click right on the center linebetween the 2 points.


Middle-clicking off the center line will result in avertical or horizontal dim, desired in some cases.





Sip

 

[rcamp]

sip's suggetsion will create and slanted dimension, but you stilll have to create a constrction line to create the angular dimension. THis is really no big deal. Constructionlines (and circles) are great technic, and allow for the creatioin of robust sketches.

 

[sip]

rcamp


Yes, you're right. Youneed toeither create a construction line or center line between the two points for the angular dimension. I'm sorry I wasn't clearer in my post.





Sip

 

[urfriend]

Thanks, It works!!