[MachFlowMike]

I'll preface my post by saying that I've read numerous beginner level posts on these forums, so I tried to do my homework before I came crying to the community for answers.

I'm very new to g-code and CNCs; I just recently got an old MAXNC set up to run on Mach3 and it seems to be working fairly well. I plan on machining mostly plastics (think plexiglass). I've been looking around for different programs to generate g-code from drawing files (I'm doing my drawing in VectorWorks which pretty much exports to any file type I can think of). I tried meshcam (which is great because it's free) and LazyCam (just the demo), and I've just started playing around with mastercam and sheetcam as well, though not in much depth. I have a few questions that I need to know before i move forward.

First off, am I at a huge disadvantage by using separate programs to draw and generate code? Will anything get lost in the import/export process? The main aspect I'm concerned with is circles/cylinders. If I were to take a cylinder (rougly the size of say a C-cell battery) and lay it on the bed of the CNC machine (so it were able to roll) could I make the machine trace the path of the circumference? If I export a file and presumably lose some of the details, is there g-code generating software that will realize that this is in fact a circle?

I'm not sure if the shapes I need to make are a bit more complicated than what is standard (I had difficulty getting meshcam to realize this and all my curves ended up very rough), but I don't yet have a grasp for what is "easy" or "difficult" for a CNC machine. The piece I'm making has to be very precise, and the curve (see attached file) must be smooth after polishing and, within reason, perfectly circular. Is this something that many people demand from a CNC machine? Am I asking too much? Is this even possible?

Any and all advice is hugely appreciated. Sorry for the wall of text. Thanks very much.

mike

[ger21]

I think MeshCAM is the wrong tool for what you're describing. Don't export 3d objects, just draw simple 2D shapes and export to LazyCAM or (better) SheetCAM.

MeshCAM will not really see a cylinder as a round object, it just sees a series of flat faces that make up the object. The higher the resolution your model is the better, but it's not 100% perfect. It can be very close, but whether or not it's good enough depends on your needs. SheetCAM, on the other hand, will see a circle as a circle. Also consider that a simple cylinder will need hundreds or thousands of lines of g-code from MeshCAM, but only a handful of lines from SheetCAM.

As for being at a huge disadvantage? I'd say no. Most people use multiple programs. It can give you more flexibility. And once you know the process that works best for you, it really shouldn't take much longer than an all-in -one CAD/CAM package.

Now, I just looked at the .dxf you posted, and something like that would be better served by MeshCAM. MasterCAM would probably be a better choice, provided that you can import the model into it as a solid, not the 3D face .dxf you have here.

[jpgdesigns]

No real disadvantage, alot of CNC programers use one software for modeling and another for post-processing. This is a very common practice.

You will only lose detail when your tooling is not a suitable size/shape to produce the detail or due to axis limits of the machine(ie. trying to cut a 5-axis part on 3-axis machine).

Just remember that a post-processor will generate a tool path for a specific tool shape relative to the geometry it is given while taking into account the number of axis the tool can move in.

Looking at the attached file, I find it does not have a smooth curve, it is made up by 8 flat faces. Most of the faces are 0.103 by the width of your slot in the part. This could be a export tolerance setting or a variable that defines the arc/curve smoothness in your CAD software. I have not used vectorworks, so not sure of a direction to point you in...

I don't know if this is important, but figured I would point it out...
Also, keep in mind that the intersection of the vertical sides and sloping an rounded bottom of the slot will not be a sharp intersection as shown in the DXF file. It will be rounded weather you use a ball endmill or square endmill. The square endmill tool would have to be perpendicular to the bottom surface on the rounded and sloping areas to achive your model. This would require 4-axis minimum and tooling long enough to reach the bottom without the tool holder hitting the sides.

Hope this helps

[MachFlowMike]

Looking at the attached file, I find it does not have a smooth curve, it is made up by 8 flat faces. Most of the faces are 0.103 by the width of your slot in the part. This could be a export tolerance setting or a variable that defines the arc/curve smoothness in your CAD software. I have not used vectorworks, so not sure of a direction to point you in...
Hope this helps

This is a DXF conversion error. Were I to export this to stereo lithography or some other extensions, that surface is perfectly round.

I realized that to do this with meshcam would require tons of code, and I knew there must be an easier way. Can you explain why, after looking at my drawing, you (speaking to Ger) would say MeshCam would still be fine? I'm also confused by your terminology, "solid" vs "3d face." I've used CAD programs for a few years, but my interaction with other users is severely limited, so there's a lot of jargon I'm unfamiliar with.

[ger21]

First, no, an .stl file would not be perfectly round. Both the .dxf you posted, and .stl files, are made up of faces. They are called 3D faces in a .dxf file. In an .stl file, the faces are triangles. Neither can form perfect shapes, because they are made up of small, flat faces. Usually, these types of surfaces are known as meshes in a CAD program. A solid CAD model does not contain "surfaces", it is a mathematically defined "solid" object. More expensive CAM programs can import solid models and create toolpaths that follow true curves. MeshCAM only reads mesh models, comprised of many faces. Because of this, it's toolpaths consist of many short, straight segments.

The reason that I said you model would be better suited to MeshCAM (vs SheetCAM or LazyCAM) is because neither SheetCAM or LazyCAM can do the curve in the middle of your part. You need a 3D CAM program for that, and SheetCAM and LazyCAM are 2D or 2.5D programs.

[neilw20]

I think MeshCAM is the wrong tool for what you're describing. Don't export 3d objects, just draw simple 2D shapes and export to LazyCAM or (better) SheetCAM.

MeshCAM will not really see a cylinder as a round object, it just sees a series of flat faces that make up the object. The higher the resolution your model is the better, but it's not 100% perfect. It can be very close, but whether or not it's good enough depends on your needs. SheetCAM, on the other hand, will see a circle as a circle. Also consider that a simple cylinder will need hundreds or thousands of lines of g-code from MeshCAM, but only a handful of lines from SheetCAM.

As for being at a huge disadvantage? I'd say no. Most people use multiple programs. It can give you more flexibility. And once you know the process that works best for you, it really shouldn't take much longer than an all-in -one CAD/CAM package.

Now, I just looked at the .dxf you posted, and something like that would be better served by MeshCAM. MasterCAM would probably be a better choice, provided that you can import the model into it as a solid, not the 3D face .dxf you have here.

This file is 3D model. Export it as ACIS.sat file then mastercam will work.

[ger21]

I think I may have given you some bad information. I should have read your first post better. You mentioned a cylinder lying o nit's side, but I messed that part. Therefore, SheetCAM would NOT work for that.

And MeshCAM is not free, btw, but they do have a timed demo.

If I export a file and presumably lose some of the details, is there g-code generating software that will realize that this is in fact a circle?

I don't think so. For reasons I mentioned above. What your exporting is seen as a bunch of flat faces. Not sure if any CAM software can interpret what something is supposed to be, when it's not.


You asked if info will get lost when exporting and importing. That depends on the format your using. stl and the .dxf type that you posted will lose some info, for reasons I've already mentioned. unfortunately, these are the formats that most inexpensive mesh-type CAM programs use. It is possible to export in a format that will not lose any info, like .sat as Neil mentioned, or a few others. but CAM software that will read those formats will cost considerably more than something like MeshCAM, usually $2K-3K and up, mostly way up.

What I'd try is to export .stl from Vectorworks, and you should have some rxport options for the .stl format. You should be able to get a much more precise .stl (at the expense of a much larger file, and more memory needed in MeshCAM) that should work OK for you. You'll probably need to use a pretty small stepover in MeshCAM to get the results you want, but you should be able to make it work for you.

[Lexx0001]

One program that you might want to look at is CamBam. It's free, and to me, it is nothing short of amazing. You can bring in DXF files and work with them. It will also take a Jpeg and convert it to Gcode and it does True Type fonts.

I can't say enough good things about it. I won't compare it to "professional" programs, (never had one, except for the crippled try before you buy), but it does everything that I want it to.

[MachFlowMike]

Thanks for the replies guys, I'll test out a few more things and inevitably post some more questions soon. I appreciate all your help.

[MachFlowMike]

I don't think so. For reasons I mentioned above. What your exporting is seen as a bunch of flat faces. Not sure if any CAM software can interpret what something is supposed to be, when it's not.

This is what I was asking about earlier. If I were to draw this figure in a g-code generating CAD program and totally avoid the import/export process, would that program realize the circular shape and generate code appropriately?

I'm starting to accept that using a MeshCam-like program will probably be my best bet. If I were making a circle (cylinder, whatever) like in the drawing, with, say, a half inch radius, how small should the stepover be to make this fairly smooth? I can always polish afterwards and do a little sanding if necessary, but of course the less of that I have to do, the better.

[ger21]

This is what I was asking about earlier. If I were to draw this figure in a g-code generating CAD program and totally avoid the import/export process, would that program realize the circular shape and generate code appropriately?

Depends on that particular CAM package.

I'm starting to accept that using a MeshCam-like program will probably be my best bet. If I were making a circle (cylinder, whatever) like in the drawing, with, say, a half inch radius, how small should the stepover be to make this fairly smooth? I can always polish afterwards and do a little sanding if necessary, but of course the less of that I have to do, the better.

The smaller the tool, the smaller the stepover needs to be. For pretty good results, try about 10% of the tool diameter.

[MachFlowMike]

I know I may be taking this post on a tangent, and if I am maybe someone can direct me where my question might be better answered: what size tool would be best for a job like this? What are the advantages of a large cutter vs a smaller one? How small is small? How large is large?

[ger21]

I didn't measure your part, but when using MeshCAM, you typically use round nose tools. This will leave a radiused inside corner in your slot. In this case, you'll want to use whatever size tool will leave you an acceptable radius in that corner. You can also try to use the Pencil Machining feature wit a smaller tool to try and clean up that corner, and do the rest with a larger tool.

For the fastest cutting, you want to use the largest tool that will give you the detail you need. You can use a larger stepover, and you get a smaller finish.

[cnc-king]

No real disadvantage, alot of CNC programers use one software for modeling and another for post-processing. This is a very common practice.

You will only lose detail when your tooling is not a suitable size/shape to produce the detail or due to axis limits of the machine(ie. trying to cut a 5-axis part on 3-axis machine).

Just remember that a post-processor will generate a tool path for a specific tool shape relative to the geometry it is given while taking into account the number of axis the tool can move in.

Looking at the attached file, I find it does not have a smooth curve, it is made up by 8 flat faces. Most of the faces are 0.103 by the width of your slot in the part. This could be a export tolerance setting or a variable that defines the arc/curve smoothness in your CAD software. I have not used vectorworks, so not sure of a direction to point you in...

I don't know if this is important, but figured I would point it out...
Also, keep in mind that the intersection of the vertical sides and sloping an rounded bottom of the slot will not be a sharp intersection as shown in the DXF file. It will be rounded weather you use a ball endmill or square endmill. The square endmill tool would have to be perpendicular to the bottom surface on the rounded and sloping areas to achive your model. This would require 4-axis minimum and tooling long enough to reach the bottom without the tool holder hitting the sides.

Hope this helps

Mastercam works great for creating the part in 2D or 3D solid and then posting the prog out to g code, that way you only have to keep control of 1 file