Help with Bolt Circle lines

[kslattery]

I am having trouble creating theALL the bolt circle lines for the pattern of holes on the drawing for the part below. I do the have the drawing option radial_pattern_axis_circle turned on but I only get a bolt circle line for the circle containing the lead element.


We make the part in many different sizes so I need it to be very flexible.


I am using 2001.


Thanks for the help.





View attachment 670

 

[CaptnPea]

Not pretty but would work,


Add datum curves that refference the center of your pattern, then goaligned withone of the axis centers on hole patterns. You can modify the line type to be phantom.


If the number of holes going out radially changes in your instances, do the curves independently, if not you can do them all as one curve feature.


Pea

 

[johncom]

ks,


Another work around would be to insert the radial center lines in the drawing. draw a circle frist then change the line type to center line.


good luck


john

 

[arroyopr]

john:


you are right about your suggestion, but you have to keep in mind that when you aren't in a 1:1 scale when you dimension the bolt circle, it's going to dimension it according to the drawing scale. Just to let know i run it to this problem before. And have use the datum curve align to circle axis works good,becuase when you modify the holes distance the curve modifies along with it. To add a little more if you don't want to show the curve on the assembly view and drawing packetjust dim. the curve then hide it and create a radial center line last it's unconvencional but works for me.


regards:


arroyopr.

 

[johncom]

arroyopr:


I tryed what you suggested. You are correct

.


I'm using wildfire and could change the curvelinetype to center line.


john

 

[skraba]

A little bit late, but still. Radial axis lines are not shown when using axis pattern. Use dimension/direction radial pattern instead to show radial axis lines in the drawing.

 

[sip]

Hi arroyopr

john:


you are right about your suggestion, but you have to keep in mind that when you aren't in a 1:1 scale when you dimension the bolt circle, it's going to dimension it according to the drawing scale. Just to let know i run it to this problem before. arroyopr.

If you relate the curve depicting the bolt circle to the view. Then it will dimension properly to scale





Sip

 

[mstols]

All these workaround are just .............work arounds.

To see the radial centre lines you need to do the following.
Set the drawing setup file option to show it. (that you've done.)

To get the desired result on your drawing you need to look at the way you created the pattern.

You need to have the angular dimension referenced when you do the pattern.

This is how you should create the pattern.(and first hole)

On a part. Start hole feature. Change references to be radial/diameter.

Select placement surface. Select secondary references. (plane and axis) complete the feature. Select the hole. Pattern using angular dimension.

Look at your drawing.

See the attached avi. (if you cant view it, download the TSSC codec from web)



2006-02-28_011445_Pattern.zip

 

[TrailBarge]

mstols,



That was a relly nice demo avi. I think that the ease with which
you pulled that off demonstrates something that I have been
suspecting for some time now:

simply put, the axis pattern is not fully functional. Going to
the old dimensional pattern solves the bolt circle problem, no sweat.



Anybody care to chime in? or should this go to another forum?



Paul P, the TrailBarge