Detail View - solid line vs phantom? What is standard? 1

[oharag11]

So, I just started using CREO and used the detail view callout tool. I was surprised that the circle drawn was solid. I asked a colleague, but we couldn't figure out how to change this. So, I went to SolidWorks to give it a go. No, SW is solid as well. You can change the line style - though it is buried deep in settings. What I didn't like is it also changed the callout line as well. Weird.

So, I have made detail drawings before - many times, and I never even thought of this issue. I have used CREO, SW and NX. So, from my memory from NX - the Detail View circle was phantom (see attached).

I don't know the ANSI drawing standard, and I tried searching for the allowable line styles for the Detail View circle. Can anyone comment? I'm posting because I want to learn.

So, you'll ask why not keep it solid. So here are my thoughts:
- I would prefer to be able to change this from solid to maybe phantom to designate the circle to be different from physical part lines. Even if I could change the line style of the circle - maybe make it bold that would be something.
- Our machinist just today asked whether the circle was a counterbore or a pocket. Yes, there is a callout flag but I still think the circle needs to be not solid.

Thanks

 

[Garland23]

It looks like the pertinent standard would be ASME Y14.2 (link below; scroll toward the middle of that page). I don't have a copy in front of me, but it should be mentioned in that one or maybe Y14.3.

https://www.asme.org/codes-standards/y14-standards

 

[Gr8blu]

For the major OEMs I have worked for, the "standard" is to use a phantom line for this kind of callout (when it HAS to be done this way, rather than a more normal section view). Not sure whether that is a take-off from the ANSI drawing standards or not, but given who the OEMs were, I suspect it is.

 

[ctopher]

It should be a thicker phantom line. In SolidWorks, it can be set in the drawing templates so it's always there.

 

[BEMPE16524]

yes it is solid line in SW. you can changed it in the setting.

 

[3DDave]

Look in the .dtl file for:

detail_circle_line_style
Sets the line font for circles indicating a detailed view in a drawing.

You can select any of the above line styles, or you can set any available system-defined or user-defined line font.
Default and Available Settings:
solidfont*, dotfont, ctrlfont, phantomfont, dashfont, ctrlfont_s_l, ctrlfont_l_l, ctrlfont_s_s, dashfont_s_s, phantomfont_s_s, cntrl_font_m_l, intmit_lww_hidden, pdfhidden_linestyle

It should also be available as an option for the drawing after the drawing is created. Note that solidfont has an asterisk, indicating it is the default so if it is not added to the .dtl file it will be rendered as solid.

 

[Sparweb]

Take Garland's advice and look up ASME Y14.2
The Phantom is a line style for generating different views.
To generate a section or detail view, one needs a line that cuts a cross-section or defines a boundary. Use lines that are dashed: long-short-short-long-short-short...

Better example is illustrated in the NASA ENGINEERING DRAWING STANDARDS MANUAL (easily found with a Google search using that title). See sheet 37.

I, too, find it annoying that the major CAD programs like Dassault don't set this properly by default.

 

[jassco]

I looked up ASME Y14.3-2003. Fig. 23 on page 14 does indeed show a detailed view with a phantom line (circle).

Best regards,