Bolt Circle

[brchapman]

Hello all,


Is there any way to add a bolt circle to a view that has holes that were not created with a radial pattern? I have a drawing of a cylindrical part with two holes in the face whose centers are concentric with the O.D. I am wondering if there is any way to manually place the B.C. Axis.





Thanks in advance for your time.

 

[prohammy]

Brchapman,


You could create a quick sketch in the drawing and then relate it to the view (a bit messy, but quick)


Kev


PS Personally, I'd go back and change the model

 

[Knut Fiskergård]

I agree with prohammy - go back and change the model. There are more benefits beyond the bolt circle - and you get a better axis on the holes.


KF

 

[arroyopr]

There is a little problem with that method. The scale factor, meaning that if you dim. that circle it's going to be base on the dwg scale. Unless is 1-1. So a work around for that is create a dtm curve on the part, then dim. dtm curve on the dwg, then hide the dtm curve. Or you can just cheet you way out by drawing a circle and add a notes. I mean there's so many ways you can skin cat in a quick and dirty way but it work.
Edited by: arroyopr

 

[pjsmith]

I would like to take it one step further than arroyopr.....create a curve on the part and when creating the holes align them to the curve, which then the curve is driving the hole placement. However, if that is notlooking for as your final dimensioning scheme, then write a relation (equal to) which controls the size/diameter of the curveand the construction curve used to create the holes.

 

[t_spraker]

I found that in WF3 if you created the pattern leader using the hole feature rather than an extruded or revolved cut feature it will automatically add the BH circle axis. There is aproblem in thatthe hole diameter dimension then shows on the drawing with 2 leaders lines across the diameter instead of the usual single arrow leader attached to the hole. To get the normal dimension I reluctantly create a drawing dimension rather than show the feature dimension.

 

[design-engine]

I do the curve in the part thing and change the linestyle too. Im going to try the method offered byt_spraker

 

[brchapman]

I guess the only way to get a B.C. on the drawing is to be sure and create the feature up front as a radial pattern. Ususally I do, but sometimes I forget when there are only 2 holes. I have used Prohammy's method for years, and was wondering if anyone had figured out an alternative. Thanks for all the input.

 

[shuga_raye]

A bolt hole circle can be added by drawingthe circle in with sketch tools in the drawing. To make sure the correct scale is used, click "parametric sketching" under sketcher preferences. To make sure the circle updates when you update attach the circle to several axes in the pattern. This is just a quick fix but it gets you the results you want.

 

[vlad1979]

I guess the only way to get a B.C. on the drawing is to be sure and create the feature up front as a radial pattern. Ususally I do, but sometimes I forget when there are only 2 holes. I have used Prohammy's method for years, and was wondering if anyone had figured out an alternative. Thanks for all the input.

Yes that's the only way but use diametral when creating the hole to be able to show the diameter of the circle, otherwise it will show the radius.


Like the others said there are some other methods, but the next best thing is Bart's method, I use it all the time when I have to make drawings with created dimensions (part of the standards of one client). Then I create a circle in part, change the line style and then I can dimension it.

 

[design-engine]

The only real drawback is that a side view may show the curve you created. Modify the created sketched curve so that you change the linetype to centerline and yellow. So just be sure to place it so the bold white lines double up with the thin yellow line.

 

[vlad1979]

The only real drawback is that a side view may show the curve you created. Modify the created sketched curve so that you change the linetype to centerline and yellow. So just be sure to place it so the bold white lines double up with the thin yellow line.

Yes but you can control that with layers, to show the curve only on one view where you dimension it.

 

[audctrl]

Create patterns like we had to in version2001 with a driver dimension. Granted the newer WF pattern tool a user can make a circular pattern from a linear placed hole. When that is done, no circular axis on your drawing, just a bunch of crosshairs.

 

[viktor_mtz]

hello all!


They can make all the options that have mentioned, use curves, sketch a circle in the drawing with parametric sketching option actived. I normally use the patterns tool to meke a circular pattern hole. And change the option radial_pattern_axis_circle to "yes" in drawing_option. This allows me, with the option show/erase to activate the axes and show the B.C. with the format axes.


I hope this is helpful to you!