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Remove lines between faces
If faces are completely tangent (and there are different degrees of tangency, just because you set your boundary surface end condition to "tangent" doesn't mean it is "perfectly" tangent) and you have the parameter in Tools>Options>System Options>Display/Selection>Part/Asembly tangent edge display set to "removed", then the edges will not show.
If you are taking the part into a drawing, and you want the edges to be hidden, you can either:
recreate the transition between the two surfaces to make it perfectly tangent (good luck!)
or more realistically, you can just use the tool in the Line Format toolbar called "hide edge". You will have to do this by hand for every edge in every drawing view.-
Remove lines between faces
Hi Charles,
I think I'm having the same problem as chris ch. I import parts reverse engineered in other software and the surfaces are all imported as separate entities. When i put it into a drawing i can still see all the individual boundary lines of each 'patch'. I tried to find the command you referred to but in the Line Format toolbar in the drawing mode, i can only find:
Layer Properties
Line Colour
Line Thickness
Line Style
Colour Display Mode
Could you point me in the right direction?
Regards-
Remove lines between faces
With the drawing view having focus, RMB and select Hide Edge. There is also a command for Show Edge.
Cheers,-
Remove lines between faces
Owen,
In addition to Anna's comments, here is a screenshot of the line format toolbar. I thought it was standard, but it may have been something I added as a customization. The button I am talking about is the one that has the two vertical lines with the red arrow. One hides lines, and the other un-hides them.
If you do this all the time (which I do), you can go into Tools>Customize, and find the buttons under Line Format. You can then add them anywhere you want, I actually have them in my drawing "S" shortcut toolbar, which I also attached as a screenshot. -
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Remove lines between faces
Chris,
As a general rule, any discrete edges or vertices between edges will propagate into adjacent faces. Our Knit command does automatically eliminate edges (eliminate topology) but if you still have edges, look at the curves or edges that exist that could be causing them. A good tool to use to simplify your surfaces is to use "Fit Spline on the 2D and 3D sketch geometry that initially creates your surfaces - i.e. if you have a profile or curve for Loft, Sweep or Boundary that is made up of a series of lines and arcs, the vertices (connection points) between the lines and arcs will propagate into the surface. Some of our surfacing features have an option called "merge tangent faces" make sure this is on if you want to simplify your geometry. Delete face and Replace face can also be used, in some situations, to "clean up" unwanted faces within the topology of your part.
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Remove lines between faces
Chris,
Try this and see if it works for you.
INSERT>FACE>DELETE>Delete and Patch (under Options).-
Remove lines between faces
Chris,
If Alan's suggestion doesn't work, you could also try and Delete and Fill.
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Re: Remove lines between faces
Hi,
i was just having this problem. Resolved by following Wingman182's comment on this reddit post:
https://www.reddit.com/r/SolidWorks/comments/599rte/how_to_remove_lines_from_merged_surfaces/
To summarise, do system options, display/selection, and change 'tangent edge display' to either phantom or removed.
Worked for me. It even contained the setting to the one part i wanted to change, and left the rest of the assembly alone. You might have to set it in the part design window (ie no assembly window) for this though.
Cheers
