propogate center marks in a pattern

Maybe I'm being 'tupid (again), but I don't remember that there IS a "propagate centermarks" function in SolidWorks. Could be a 2004 thing (I haven't taken the plunge yet), but as I presume you must be dealing in a Drawing I also presume you have HOLES, or at least radii, where you want centermarks. If that be the case, then all you need to do is go to "Tools" -> "Options" and in "Document Properties" under "Detailing" check the box under "Auto insert on view creation" labelled "Center marks". The go back to your drawing and insert your view again in which you want the center marks to show up.

'Sporky'

Rollie wrote:

Rollie

The Propagate Centermarks button pops up automatically adjacent to a selected hole when you've got either the Linear Center Mark or Circular Center Mark selected in the Options box of the Center Mark Property Manager, and I would assume when SolidWorks recognizes the hole is part of a pattern. This is what I think is going on anyway - there is no Propagate button on any of the Toolbars I've seen...

I'm also drawing a blank here. Will you, please, run me through an example step by step to be able to see what you are talking about?

I do kind of remember a macro that would put centermarks on all circles on a selected face in a selected drawing view. I can look for it if desired.

WT

In a drawing of a part with a hole pattern (circular or linear)....pick the Center Mark tool, pick Linear Center Mark or Circular Center Mark in the Options box, then pick the edge of one of the patterned holes. A little blue button pops up that looks like a reversed Offset Entities button. Click it and all the holes in the pattern are filled in with center marks.

Thanks - it's amazing how something as simple as that can go unnoticed. I had seen the icon before, but never stopped long enough to investigate.

WT

Just tried the options there. It appears that unchecking the "Base Center Mark" box does not stop the insertion of a central centermark. Am I missing something?

WT

Good Morning,

Thanks for your help! This button will pop up in a drawing when the hole has been created as a pattern only. On plates, using the hole wizard, I have holes in linear patterns but most of the time these holes are not equally spaced, so I can't call these a 'pattern'(unless I rename them?). Thus, in a drawing the propogate centermarks button does not open. I can still connect with linear centermarks (horizontal & vertical) I just have to do more clicks. My next question is the connection line font - anyone care to guess on how to modify the font? I mean the font does not scale itself when printing a plot. On a 22 X 34 drawing, the font practically disappears.

In 2004, using the Hole Table for my purposes will really speed things up.

Hey 'Sporky' don't feel bad about being "'tupid", you are not alone.

Rollie

Wayne -

If you are, then I'm missing it too. Checking the option does not seem to make a difference. Wonder what it's there for?

SWX 2004 has fixed the scaling of the connection line font between centermarks, regardless of ISO or ANSI settings; now the line looks the way its 'sposed to...

Rollie

Here's what I see about propagating center marks - try it out and see if you get the same results. I'll submit it after a few more people try it to see if it's consistent.

1. Create a part with a circular hole pattern in it.
2. Create a drawing with that part in it.
3. Start the center mark tool.
4. Uncheck the "Circular lines" & Base center mark" boxes.
5. Select one of the circles in the drawing and click the propagate icon that appears next to the circle.
6. Notice that the base center mark appears anyway.

Notes:

1. You can always just delete it if desired.
2. If you go back and check/uncheck any of the boxes, they appear to work properly.
3. The other 2 boxes appear to work as expected.
4. SW2004 SP0 works the same way.

WT