Bolt Circle on a Drawing 1

[markbreneman]

I'm trying to make a dimension of bolt circle on a drawing and I'm looking for some help. Any tips?

 

[ttx]

markbreneman,

You can create a datum curve in your model.
Change the linestyle in your drawing to match the drafting standard that you are using.
You can also rotate the the hole axii to match the BC.

Hope this helps.

Cheers,

JW

 

[Mike97D]

I use a different method when wanting to make a bolt circle type dimensioning scheme.

I start by making a sketch for locations of the holes for the extrude function. On the sketch I will use a circle to start for the BCD and right click to change it to a construction circle. Then add the holes as needed using the construction circle for their placement. Finish the sketch, make the extrusion and select cut. In drawing mode, show dimensions, make note of the id number (dxx) [either by switching dimensions or selecting the dimension properties] for the construction circle and add it to the actual hole dimension under properties in the text area/tab. You'll have real dimensions in your shown dimension on the drawing that will be editable.

The one negative of not using the hole funtion is that this method does not give the drill point cause your using extrude.

Hope this may help,
Mike

 

[vc66]

If you're using WF2, you can go into your drawing setup file, and insert the following...

radial_pattern_axis_circle yes

Now when you create your hole, and pattern it, use the "radial" option, and when you show your axis on the drawing, it will automatically show the Bolt Circle along with the angled hole axis.

I don't know if this works in other versions.

V

 

[TCGT]

When you create the hole, use the diameter option within the hole tool. This option will require you to specify the initial angle and bolt circle diameter. You can then pattern hole using the angle dimension.

In your drawing, show all axis and the axis of the bolt circle will be shown. In addition, when you show dimensions for the holes, the diameter of the bolt circle will be shown and pointing the bolt circle axis.

I hope this helps.

 

[markbreneman]

Thanks to all the help. I tried the above options, which all work for typical bolt circles, bu the geometry i had was not an actual bolt pattern but more a bunch of triangular points which fell in a circular pattern. I ended up just placing a sketch in the part, on a layer, and then adjusting all the views on the drawing i wanted to show the layer or not. thanks for all the help though.

 

[mmuell01]

Most software packages do this easily, usually with a single click

Option 1 for Pro E:
Print drawings, add bolt circle centerlines by hand and scan image.
Option 2 for Pro E:
Use UG, SDRC, Auto(cough)Cad or SW.

Anything having to do with hole centerlines on a drawing is extra work. Also why does pro e break circle into 2 segments with no pickable centerpoint? Very weird.

Good luck

Clickin' like crazy in Pro E

 

[franzdom]

mmuell01, if you want to add centerlines to entities that don't have them, you can add an axis in sketch mode, then show the axis in the drawing mode. Also, centerpoints can be selected, are you dimensioning when trying to pick them or ??