CAD and dxf file experts, get in here.

[oxford]

I have some DXF files of flat layouts for a set of pipes.  I opened up the "large cone" file in autocad.  While playing around I noticed that the "ends" of the cone weren't a true radius in the flat layout and were made up of a bunch of "straight" lines as best as I could tell.

It this something that happens when the original drawing gets converted to a DXF file or would it have been drawn like this originally?

I split the cone in half using true radius as my slip roll can't handle it full length.  I printed it 1:1 on paper and can't see any difference from the true radius line and the segmented one.

I was just curious as to what was going on.

[Striker1423]

how zoomed in were you in the cad software?

[Vintagetz]

It depends on how the flat was generated, there is a chance that the "curve" required to replicate the end of the cone in the flat was actually a spline, not a true arc.  There are no flat-cutting machines that can cut a spline, they are normally converted to line segments or connected arc segments. 

On some systems when a spline is converted there is a conversion tolerance, this is what dictates the line/arc segment lengths.  The tighter the tolerance the more segments there will be.  I can take a look at it if you would like me to.

I will PM you.

[oxford]

how zoomed in were you in the cad software?

First off, my CAD experience is not very much.  I was pretty zoomed in when you could see it but I noticed it first when I couldn't measure the "radius" using the measure function.

I was more curious than anything as I had this file cut out before and nothing was said about any issues with it.

[oxford]

Thanks vintagetz, for the little I know, that makes sense and most likely is it.

[Striker1423]

I was just wondering, because every car part I ever looked at digitally was the same way when zoomed in super close.

[m in sc]

what you see on the screen isn't always what you have.... I have 25 yrs experience in drawing, but don't use inventor or most autodesk stuff anymore, usually solidworks.

anyway, export functions, etc, will determine how the curve is interpolated. usually, true 'arcs' aren't usually displayed when zoomed in super close on a .dxf. however, if you save that file as a PDF it will create it as an arc, for example.  odd you couldn't measure it, it may have been converted into a series of straight lines, not uncommon in going from different file types to different software's back and forth... but can be over ridden usually in display or output/export settings. you can always trim out the straight sections and re-fillet the curve but it probably wont matter in actual functionality/output  . but vintage tz is pretty spot on on his explanation. 

[oxford]

It would let me measure distant on the sections, it just wouldn't measure as a radius.  I guess obviously now since it wasn't.

[Vintagetz]

I have 38 years of experience and used to work for a CAD/CAM vendor in the EARY days of 3D and 3C surfacing/machining. 

The following is fairly technical but it can help anyone interested to understand the issues being raised in this thread.

First it is very true that some graphics cards or even the software will show an arc as line segments if you zoom in far enough.  To know if this is the case all you have to do is inspect or analyze the entity, the cad software will tell you if it is a line or an arc.

When you export a file what you get depends on what you start with and also the format and version a file is saved in. For example, DXF files are actually text files.  The first version was 2D only, DXF then evolved into 3D, but it was still just lines and arcs. 

Splines are variably geometry entities, think of them as a constantly changing arc, where the radius changes along its length.

There are multiple different formats for CAD and 3D surfaces and 3D solids.  I'll try and give you an idea of what the file types are, and what can be done with them.

Definitions:

Native Format:

This is the internal file type for a given CAD or CADCAM system.  For Solidworks, The extension is .sldprt, for AutoDesk Inventor (AutoCads 3D) the 3D file is a .ipt, For "AutoCad 2D" the native format is a .dwg.  Virtually every cad system has a "native" or internal format file structure.

Native format files contain data that is internal to the Cad system, meaning details that represent more than just the shape of the part/design.  Most companies publish their native file formats, this allows me to open an Inventor "native" file in Solidworks. It does not mean I get 100% of the data, there can be differences and in this case, I will get a notice that some entity types are being converted.

Neutral Format:

This is a format that allows different cad systems to transfer data,  not 100% of the native information/data is supported.

DXF is a "Neutral format"  it was designed to allow the transfer of data between two differing cad systems.  It is actually a text file, you can open it in word or notepad, or any program that can display a text file.  What you will see is a series of coordinates and instructions, like a line or arc.  Think of it as a macro that tells the CAD program how to draw the part. As the DXF format has expanded additional features have been added such as 3D support, BUT it is a line and arc program, that is all you will see on the display.

STEP and SAT are 3D surface / 3D solids neutral formats that allow a 3D part to be transferred between two different 3D systems.  Again not all details are transferred, The most significant are 3D sheet metal designs that are created in the sheet metal or fabrication modules.  These types of parts can be unfolded by the 3D software based on the growth parameters for any given material.  None of the neutral formats support unfolding.  This means that a sheet metal model from Inventor that is saved as a  STEP or SAT has to be converted into a sheet metal model if it is to be unfolded.   This conversion can take almost as much time as just redrawing the part from scratch.

Much like the example with 3D sheet metal parts, there are entity types that are not supported in DXF, splines have been one of these.  It has been a while since I looked at what is supported in the latest version of DXF so I am not sure if splines are supported or given the limits of the DXF format they will ever be supported. 

What I do know is that no flat-cutting CNC machines (laser, plasma, waterjet) control support cutting a spline so the CAM output will create a series of connected line or arc segments that simulate the spline. 

Most cam systems allow you to specify an "output tolerance"   This value is how far the segments can deviate from the true shape of the spline.  For example, if I say it cannot deviate more than .002"  no part of the line or arc generated will deviate from the true shape of the spline by more than .002" Keep in mind, this does not mean that any two points along the path will be within .002 of each other relative to the original geometry, that value would be 2 X .002" or a maximum deviation .o .004" for the output lines or arcs from each other (a spline can be a single "S" shaped entity).   So depending on the direction of the spline there could be a segment that was -.002 from the true position of the spline while in another area there could be a segment that was +.002" from the true spline position.

How the output tolerance impacts what is created is directly related to the number of entities required to generate the profile, the difference between an output tolerance of .001 and .005 can be big as far as the number of lines or arcs needed to create the profile, example, .001 could generate 1000 segments where .005 could generate 120.

For me this falls into the category of the fly shit and the pepper rule, there is a tiny amount of fly shit in the pepper, and it's not worth trying to pick it out, Meaning that the lines do an incredibly good job of accurately creating an arc that can be cut.

Unless the output tolerance is set to .060 or more the fact that the arc is represented by a series of line segments is not measurable or detectable. If the output allows the use of arc segments it is even less detectable.

[Vintagetz]

If you want to get an idea of the radius of an arc that is represented as a series of connected line segments you can draw lines perpendicular to each of the end lines starting from their endpoints and extend them until they intersect. The length from the entity to the intersect will give you the approximate radius.

you can also create an arc if you want to see the deviation,  construct an arc with an unknown center that begins and ends at the starting and ending line endpoints (at both ends of the series of segments)  then specify that the arc to be constructed is tangent to a middle segment,  the system should generate an arc according to those rules.  You can then zoom in and measure the deviations, and if they are significant you will see the difference immediately.

[oxford]

This is some interesting stuff even if it is a little over my head.

Who sets the "output tolerance"?  Cutting operator when they load the DXF file or is it set when the original file is converted to a DXF?

From above it sounds like it's the cutting operator.  If it is, what would be the advantage for them of putting in a big tolerance vs a small one? 

[Vintagetz]

It is set when you output the geometry to the DXF file.  Setting the tolerance really close greatly increases the number of segments and can REALLY SLOW down the cutting.  Honestly once a cone is rolled you can't see its line segments unless they are inappropriately long.   Someplace in my backups, I have an MSDOS-based program that creates DXF cone segments.  The input is inlet diameter, outlet diameter, centerline radius, and total sweep angle.

The faceting occurs when you are outputting the flat of a cone that has an angled cut on both ends.  The flat shape of the edges sort of looks like an untied bow tie, it is called a sinusoid. It is what creates those beautiful flawlessly smooth segmented pipes. They are not rolled as a straight cone and then cut into segments and rotated, each segment is an individual tapered cone with angled ends after it is rolled.

I have two sets of SS RD400 pipes that cross over in front of the motor and then exit GP style. (need to get my welder going again and finish them).