My question is, If you are detailing a drawing, in the standard 2-D views is it acceptable to leave the tanget lines visable on the drawing. With the Iso view this is common practice but I believe it is becoming more of an accepted practice. Can anyone confirm what I'm saying or am I incorrectly detailing 2-D drawings?
Eng-Tips is the largest engineering community on the Internet
Intelligent Work Forums for Engineering Professionals
-
Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!
Tangent lines permissable on a 2-D drawings?
- Thread starter tomlab
- Start date
MikeHalloran
Mechanical
I used to shade bends with parallel lines of graduated weight, when that was just a matter of keeping two or three pencils in your hand. The last, very light, line was usually near where a tangent line would be. The lines were usually broken in some way so they wouldn't be confused with object lines. I thought it added clarity for little expense, and reproduced better than the shading available in CAD.
I'm not real thrilled with having tangent lines or nothing as the only options, but the tangent lines add clarity. ... sometimes.
I don't know what the various standards have to say about it.
Mike Halloran
Pembroke Pines, FL, USA
I'm not real thrilled with having tangent lines or nothing as the only options, but the tangent lines add clarity. ... sometimes.
I don't know what the various standards have to say about it.
Mike Halloran
Pembroke Pines, FL, USA
Per manual drafting practices that was not acceptable. Imaginary lines were used instead. I've repeatedly asked our CAD supplier to implement imaginary lines to no avail. I can draw them easily, why can't they?
I don't like tangent lines but I will sometimes turn on one or two in an orthographic view that looks like an unintelligible blob without them. Some times I'll draw in the imaginary lines but that kind of defeats the purpose of parametric solid modeling. I don't even show all tangent lines in an iso view as there tend to be way too many and our iso views are usually small.
I don't like tangent lines but I will sometimes turn on one or two in an orthographic view that looks like an unintelligible blob without them. Some times I'll draw in the imaginary lines but that kind of defeats the purpose of parametric solid modeling. I don't even show all tangent lines in an iso view as there tend to be way too many and our iso views are usually small.
- Thread starter
- #4
Mike,
My thoughts exactly, but I have a co-worker that is 2 decades earlier than myself, and I do believe that this type of drafting was frowned upon at that time. With that being said and having to work with other countries, the more information that you can put on a drawing the better. It closes that door for interpretation, which in our case could be in the tens of thousands of bad parts.
My thoughts exactly, but I have a co-worker that is 2 decades earlier than myself, and I do believe that this type of drafting was frowned upon at that time. With that being said and having to work with other countries, the more information that you can put on a drawing the better. It closes that door for interpretation, which in our case could be in the tens of thousands of bad parts.
- Thread starter
- #5
dgallup,
I do remember during my manual drafting days that you are correct and it was a way of not blurring the views and making them hard to visualize. We use Solidworks here for our CADD package and I think that the program does a real good job of making the drawing views very clear.
I do remember during my manual drafting days that you are correct and it was a way of not blurring the views and making them hard to visualize. We use Solidworks here for our CADD package and I think that the program does a real good job of making the drawing views very clear.
Not sure what the standards explicitly say, but my rule of thumb is that if it adds clarity or somehow makes the drawing easier to understand then do it.
If it may lead to confusion, or a messy/busy/crowded... drawing, leave it off.
Put the minimal information required to explicitly define things - less is sometimes more.
Before I bother looking, what drawing standards, if any, do you work to?
If it may lead to confusion, or a messy/busy/crowded... drawing, leave it off.
Put the minimal information required to explicitly define things - less is sometimes more.
Before I bother looking, what drawing standards, if any, do you work to?
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
Only show lines that are needed to convey any details of the part. Otherwise leave them off to reduce clutter.
Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion
Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion
- Thread starter
- #8
ASME Y14.2 may be the one you need to look at, which sadly I don't have a copy of. Y14.3 doesn't say that I can see.
I'd look in Genium or Global but don't really have the time right now.
I'd look in Genium or Global but don't really have the time right now.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
MikeHalloran
Mechanical
I love Solidworks for modeling, but I don't care for the drawings it produces. They have a distinct style, which means they can usually be interpreted in a consistent way, _if_ the viewer is used to it.
Adding clarity requires dealing with SW's drawing editor, which I _really_ hate, mostly because it actively fights doing anything in a way other than whatever the hell way Dassault thinks things should be done. There must be some Gallic logic to its schizophrenic behavior, but so far it eludes me.
Mike Halloran
Pembroke Pines, FL, USA
Adding clarity requires dealing with SW's drawing editor, which I _really_ hate, mostly because it actively fights doing anything in a way other than whatever the hell way Dassault thinks things should be done. There must be some Gallic logic to its schizophrenic behavior, but so far it eludes me.
Mike Halloran
Pembroke Pines, FL, USA
- Thread starter
- #11
Solidworks, I have to agree modeling is the fastest program I have used to produce functional 3-D virtual assemblies. But the drawings are so open to what they interpret that I am always changing something to try and keep within the standards.
Tom - automotive
Virginia
Tom - automotive
Virginia
We use ISO standards so this is not exactly relevant. But, FWIW, ISO 128 section 3 lists all the types of lines and how they should be drawn. Tangent lines do not appear anywhere on the list but imaginary lines do. Section 5.2.2 goes on to say:
"Imaginary intersection lines (such as fillets or rounded corners) may be indicated in a view by means of continuous thin lines, not touching the outlines."
I don't know of a single solid modeling system that can automatically produce those lines. I can manage to fake it sometimes & keep associativity with the model if I have dimension lines to sharp corners that were subsequently rounded. I can drag & break the dimension leader line so it can also make an imaginary line.
We really should beat up on the CAD companies to get them to implement this functionality. I'm sure they could if there was enough demand. They implement tangent lines just because it is easy for them to do so but they really have no place in proper drawings.
"Imaginary intersection lines (such as fillets or rounded corners) may be indicated in a view by means of continuous thin lines, not touching the outlines."
I don't know of a single solid modeling system that can automatically produce those lines. I can manage to fake it sometimes & keep associativity with the model if I have dimension lines to sharp corners that were subsequently rounded. I can drag & break the dimension leader line so it can also make an imaginary line.
We really should beat up on the CAD companies to get them to implement this functionality. I'm sure they could if there was enough demand. They implement tangent lines just because it is easy for them to do so but they really have no place in proper drawings.
MikeHalloran,
I agree that SolidWork's 2D drafting is adequate, rather than excellent. My 2007 version has the option of adding tangent lines has heavy, solid line, or as thin phantom lines. I add the thin, phantom lines when I think it will make make drawing clearer.
I mess with line thicknesses when I think it makes the drawing clearer. This includes side views of chamfers and other oblique angles, and it includes foreshortening of parts with messy front and rear features. Back in the old days, on a drafting board, I would break the distant lines as they approached the lines of the front features. There is no convenient way to do this in SolidWorks.
JHG
I agree that SolidWork's 2D drafting is adequate, rather than excellent. My 2007 version has the option of adding tangent lines has heavy, solid line, or as thin phantom lines. I add the thin, phantom lines when I think it will make make drawing clearer.
I mess with line thicknesses when I think it makes the drawing clearer. This includes side views of chamfers and other oblique angles, and it includes foreshortening of parts with messy front and rear features. Back in the old days, on a drafting board, I would break the distant lines as they approached the lines of the front features. There is no convenient way to do this in SolidWorks.
I dont know About Standards But We some time Use tangent lines for dimensions.Main Reason for this is to get actual Width and Length of Part.This width and leng are later added during BOM creation.(Mainly we use this for Sheet metal parts where Laser cutting done using Huge Sheet metal part to create diffrene Flat patterns).
*Some time Intersection also used
NX 6.0.2.8 MP4
Teamcenter 2007
WINDOWS XP (64 Bit)
*Some time Intersection also used
NX 6.0.2.8 MP4
Teamcenter 2007
WINDOWS XP (64 Bit)
CheckerHater
Mechanical
dgallup: "I don't know of a single solid modeling system that can automatically produce those lines."
SolidWorks does. Check "Hide Ends" in "Tangent Edge" settings. Unfortunately only works for straight edges, revolved features are not supported yet.
And Mike, about "schizophrenic Gallic logic".
Solidworks is located in Concord, Massachusetts.
SolidWorks does. Check "Hide Ends" in "Tangent Edge" settings. Unfortunately only works for straight edges, revolved features are not supported yet.
And Mike, about "schizophrenic Gallic logic".
Solidworks is located in Concord, Massachusetts.
CheckerHater: Tangent lines are NOT imaginary lines. Tangent lines come in pairs, at each end of the round. Imaginary lines are singular per round. Also, imaginary lines are most useful for revolved features.
Re "schizophrenic Gallic logic" Salidworks is owned by Dassault, a French company.
Re "schizophrenic Gallic logic" Salidworks is owned by Dassault, a French company.
CheckerHater
Mechanical
I agree.
Some shapes may be better off dimensioned to tangent line, but if "sharp corners that were subsequently rounded" are your game, SolidWorks calls them "virtual sharps"
No need to fake anything.
Some shapes may be better off dimensioned to tangent line, but if "sharp corners that were subsequently rounded" are your game, SolidWorks calls them "virtual sharps"
No need to fake anything.
Those are not imaginary lines either. In that image, an imaginary line would extend from just short of the left & right sides at the .239 & .471 heights. In Pro/E I can drag the dimension extension lines across the part and then place breaks in them to make what looks like imaginary lines. These will behave parametrically if the height changes. However, if the diameter changes I have to manually drag the break points around. I know the CAD systems could do it, they just don't even try.
CheckerHater
Mechanical
Thank you dgallup,
I understand what imaginary lines are, I just feel uncomfortable with using the word "fake" next to "dimension", and I was trying to point out that until software companies start do things your way, there is an alternative that allows you to dimension with precision.
I understand what imaginary lines are, I just feel uncomfortable with using the word "fake" next to "dimension", and I was trying to point out that until software companies start do things your way, there is an alternative that allows you to dimension with precision.
- Status
Similar threads
- Locked
- Question
- Locked
- Question
- Locked
- Question
- Locked
- Question