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parametric sketching in drawing

sbpanda

New member
Dear All


Can u pl tell me how to sketch ,take an instance ,,Suppose I have a model of round solid cyllinder & at its one face there are 16 nos holes, i want ot sketch a construction center line ,taking the cyllinders center as the const. circle's center & the periphery of the const. circle should match with the ceter of the holes.


View attachment 667





thanks
Edited by: sbpanda
 

maxweston

New member
Hi Sbpanda,


I assume by your explanation that you want to be able to display a pitch diameter circle thru an existing array of holes, if you do then create a datum sketch in the form of a circle using your component axis and the axis of one of the 16 holes.


Once you have the datum sketch created select it and right click, select properties and change the line type and color to what ever you need.


Regards,
Max Weston.
 

sbpanda

New member
Dear Maxweston


Thank u very much for ur reply, this also i know, but when u will creat views in drawing mode, the center line will also visible in other views(side & all), but this i don't want.


Can pl help how to draw the same as i mentioned in the top view only, I mean it should not visible in other views.


thanks & regards


sbpanda
 

puppet

Moderator
if u create ur holes from the "hole tool"

then patterned them along ur diameter.



then in ur drawing if u goto show/erase and then pick
centerlines. it will show u ur pcd aswell. (drawn automatically
as a construction line)



is that what you mean?
 

sbpanda

New member
Mr Puppet


thanks for ur reply , I got what i wanted, but if i am not done it in hole option as these are the blind holes & at the base of the blind hole there is some profile.


And I made it by tweak-offset then pattern it. In this case how to get the centre lines as I mentioned above in figure.


thanks & regards
 

dr_gallup

Moderator
Set radial_pattern_axis_circle to yes in your drawing setup dtl file. Then you can control display fo the axis through the show/erase dialog box.
 

donha

New member
You sometimes have to use cosmetics or datum curves to display as centerlines. With either of these options you can change the line style in the part. The other option is what Dr stated.
 

sbpanda

New member
Dear dr_gallup


What u explained i tried that but it is not showing, i think as i make it by tweak-offset option, the center axis for individual blind holes are not present , should i make axis for all the 16nos. of blind holes, then should i try ur tips.


regards


sudhanshu
 

dr_gallup

Moderator
If you can not get Pro/E to display the bolt circle the way you defined the features, then it is easier to just use a cosmetic feature(s) to show the bolt circle. I find cosmetic features better than datum curves because you can control their view display more easily through the show/erase dialog box.
 

sbpanda

New member
Dear All


Igot it what i wanted, i.e. , go to sketch tools--construction circle--use ref snaps--draw the circle taking the center of the existing model circle and then snap at the hole center point.


thanks for all of ur supports.


sudhanshu
 

robertib

Member
Another way of doing this is to make a sketch, using the centre axis & outer axis as the references, then changing the line style to centreline (through properties).
 

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