Router Forums banner
1 - 12 of 12 Posts

·
Registered
Joined
·
6 Posts
Discussion Starter · #1 ·
I have had a long time desire to own a CNC Router and make stuff. I'm sure that is one thing everyone here has in common we all like to make stuff.
When I search CNC routers I find tons of videos of cool stuff being cut at 100x speed and then showing a finish product. I find very little showing all of the extra steps and work that goes in to it all, and almost nothing on software. I do not have a machine yet and am more concerned about starting right (for my needs) versus starting fast or as inexpensive as possible.
My first thing that I need to understand is software and what the gap is between my desires and my capabilities. I have no cad experience.
I want to be able to import logos and cut them 2D for signs. I want to be able to import grayscale and have it cut in 3D. I want to import a pattern and have it cut. I do not have a desire to trace or re-draw the imported items.
I will want to be able to nest projects. If I have a small size popular piece that will be cut more than once, I do not want to need to set up over and over if 10 will fit on the table.
I am even interested in a vacuum table if it mean I do not need to go back and manually cut away where the hold downs are and I can cut away 10 finish pieces from 1 piece of material.

Is all of this possible?
I appreciate all suggestions and advice.
 

·
Registered
Joined
·
4,380 Posts
Sounds like a candidate for Vectric Aspire or Vcarve, don't cha think, guys??

Go to Vectric.com and download their trial version of Aspire or Vcarve and you can do anything the software will do - - except download files. It's free and it will give you a feel watching their tutorials and using the real thing. Then decide what you want to do.
 

·
Registered
Theo
Joined
·
7,194 Posts
I want to be able to import logos and cut them 2D for signs. I want to be able to import grayscale and have it cut in 3D. I want to import a pattern and have it cut.
You will have to be cautious doing that, and avoid copyright violation, that could get expensive.

And that's about all I know about CNC, or want to know, wouldn't have one.
 

·
Administrator
David - Machinist in wood
Joined
·
4,196 Posts
Another thing to be cautious of, Scott, is when you import a jpg (or other) file there are frequently tons of nodes that can slow your process and/or increase your cutting time. I usually import into CorelDraw, reduce the nodes or clean up the lines, and then export that as svg so I can bring it into Fusion 360. Maybe the Vectric line of software allows direct import of jpg files but the ones I have played with are not very clean.

Copying or repeating an item multiple times shouldn't be an issue at all and for light production items it certainly makes sense to do it that way. Vacuum tables are very useful, as well.

From your wish list it sounds like you want to take images off the 'net and go straight to cutting with few steps in between and I don't know that that is possible, at least not as simply as I stated it. Be sure to keep us in the loop with what you choose so we can learn and check this out, as well.

David
 

·
Registered
Joined
·
1,586 Posts
Excellent questions that will benefit all of us out here who are strongly considering taking the plunge into the CNC world. I look forward to the discussion they generate. Thanks.
 

·
Registered
Joined
·
218 Posts
Excellent questions that will benefit all of us out here who are strongly considering taking the plunge into the CNC world. I look forward to the discussion they generate. Thanks

+1 to that
 

·
Premium Member
Joined
·
201 Posts
I have 30+ years experience using AutoCAD. For me the move to using VCarve Pro & Mach3 was still a little challenging. You can find the answer to just about any problem you have learning most software for cnc control & programming on You Tube. Don't get frustrated if you download the trial version of these software packages, take advantage of all the experienced users online. There are forums for most cnc software.
 

·
Registered
Joined
·
6 Posts
Discussion Starter · #8 ·
If we assumed That I of course received the necessary permission for this image (this is just an example image), is there a program that will allow me to import this and have the different colors of gray cut as different depths so it comes out as a textured or 3D image? I have seen these cut out on YouTube but I do not yet understand how to go from the grayscale image to the finished product? Can anyone help enlighten me?
 

·
Super Moderator
Joined
·
5,816 Posts
Like mentioned, Vectric's VCarvePro or Aspire will allow you to import the image. Then you can trace it. At that time, you will need to clean up the image as needed. You may be able to answer your own questions by browsing the tutorials Vectric has on You Tube.

Download the trial version and start learning how to use it. You don't need a CNC to use the trial software. That is what I did and it worked OK for me.

Good luck.
Mike
 

·
Registered
Joined
·
6 Posts
Discussion Starter · #11 ·
Mike,
Thank you for the response. I appreciate the help. Before going out and buying a laptop and a router I am trying to understand the capabilities with my not having experience. When you say trace, do you mean that you need to redraw every line and set different layers? I was under the impression that there is a way to import the grayscale as a certain file type and the software will automatically make each different gray color a different layer. I am trying to understand can you simply import, save as a certain file type and issue a command to cut?
Does the software decide when a roughing bit is need and when a finishing bit is needed, or do I need to know how to program that?
 

·
Registered
Joined
·
376 Posts
This will be a long post. Its late for me, so I will try to add some examples and links to specific youtube videos or tutorials in a later post.

There are several types of images and types of carvings that can be created from them, depending on the software you are using. Generally you cannot rely entirely on software to do everything for you - for every image type you will need to provide some context as to what you want. For example, most image formats do not include any size information - do you want that image carved 10 inches or 3 feet across. In most software, that is one of the first steps, choosing the size of your workspace. The software will generally allow you to resize the image to fit the output size you want.

After reading below - I urge you to follow the advice above and use a demo of several software programs and try each type of image - most of the programs have tutorials for some of the types of image below. Usually there is some sort of 3D display that you can rotate on screen to get a sense of what the carving will look like, and often a “simulation” where you will see the bit moving around and removing material like the CNC will, starting with a simple block (you will define the “stock” size the machine will start with) and ending with the finished part. You will also choose a point on the stock (often a corner, or the center) that is the origin that represents X0, Y0 and Z0.

1. CAD file. This is where you specifically design something you want cut in full 3d. For example, the body of an electric guitar. There is a “profile” or outline of the part, and there are “pockets” or areas carved to different depths, and there may be holes, which might be through holes or just to a certain depth. The CAD file contains the full definition of the part - but you will still need to add context to instruct the computer when doing the CAM part - creating toolpaths or the instructions for the CNC. For example - what size bit will you use to cut the outline, how deep will you cut on each pass around the outline, will you leave tabs connecting the cutout part to the rest, etc. Often you will choose to use multiple bits, perhaps a large diameter one for larger areas (roughing) and a smaller one for more details (such as smaller holes or radiuses). Fusion 360 is an example of a program you can use to do both the 3D design of a part and the CAM portion in one program (free for hobbyist or under $100K/year commercial use).

2. Vector image - for example an image created in Adobe iIllustrator or Corel Draw, an "SVG" image downloaded from online or even a DXF file exported from AutoCad or other programs. Think of words or logos. These can be imported into software such as V-Carve pro ($799), Aspire ($2000) or ArtCAM ($360/year), or f-engrave (free) and you will be able to create toolpaths. Here the context you are adding is if you want the image raised (background cut away), or recessed ( the image cut to a certain depth) and by how much or if it is a line image, carving along the lines (V-carving). You can create this type of image directly in this software as well. The “vectors” are mathematically defined - there is no “dots” or pixels in the image - smooth lines and curves as far as you zoom in. You also need to choose the size of bit you are using (large bit for big areas, smaller for more detail. For V-carving you will need to decide on the angle of the V - bits are available from 30º - 120º. Different angles will have a major impact on the appearance of the carving.

3. Monochrome or a few solid color bitmap. This could be a black and white image - on the screen may look just like the vector images - text or logo etc. But if you zoom in, you will see that the image is make of dots or pixels. These can be imported into these same software titles and “traced”. This means the software will “outline” or create vectors from the bitmap, and then you proceed as in #2. Usually the program will do each solid block as a separate closed vector (outline) in one quick step.

All of the items above are carved as vectors - series of curves and straight lines. G-code only handles straight lines and arcs - the software doing the CAM will approximate any other type of curve using straight lines and arcs. You can usually assign a tolerance value - how far the approximated path of the tool can deviate from the mathematically perfect path. The smaller the tolerance, the more little straight lines and arcs are used. You will see the CNC move directly around your machine like the curves on the screen look.

The next image types are carved differently - they are raster image formats and get carved like an inkjet printer prints - you will see the router go in parallel lines, back and forth, with the Z axis going up and down. This can be very time consuming, depending on values you will set for the size of the bit (usually a ball end bit - so the diameter ) and the “stepover” or distance each row is from the previous - usually defined as a percentage of the diameter of the bit you use. The smaller the bit and stepover, the more rows of passes and the longer it takes. The more detail the better it looks The G-Code itself is still just lines (usually no arcs) - they are just lots of short moves across and up and down.

4. Bitmap images designed specifically for CNC carving (reliefs). These are special grayscale images that are set up so that the color of each pixel encodes the relative height of that point. For example a light colored pixel will high, and dark low. Again, you need to provide context in the software - what distance do you want between high and low - 1/8 of an inch or 1 inch? Think of a topographic map, where the color reflects the altitude. There are sellers of these images or they can be created by 3D scanners. Often these reliefs can also be created directly in programs such as Vcarve, ArtCAM or Aspire by operations such as extruding a vector or sweeping a vector along another one, or revolving one. Even though these are mathematically created shapes - they get carved in the row by row format. Autodesk has free software for smartphones that can create a relief from a series of pictures you take of a physical object from multiple angles. Lets say if you have a carving you need to reproduce.

5. A standard bitmap image (photograph, etc.). The software will attempt to analyze the image and create a relief - some programs do this better than others trying to infer relative hight by analyzing shadows - some just treat light areas as high and dark as low. Some images work very well, others do not. The tiger image you linked to would probably not work very well without some work (isolating the tiger from the grass background, etc.)

Others may be able to add additional formats, but I believe the above are the major types. As you can see - for every type of image you start with (or create) there will always be something you need to define or do to create the toolpaths.

Finally, the toolpaths (expressed as a g-code file) gets loaded into your machine control program (such as Mach, WinCNC or LinuxCNC) these are the programs that execute the g-code and actually operate the CNC. This program will need to be configured specifically for your CNC. You need to set up things like how many discreet "steps" it takes for each axis to move 1 inch (or mm), and how fast your machine can move (inches per minute). If you buy a machine, the manufacturer should preconfigure this for you. If you build one, you need to do this yourself. This is generally a one time operation.

Finally, you will need to locate the stock on the table of the CNC and set up the machine to the same origin that you defined way above when you started (remember that X0, Y0 and Z0?). Then and only then will you be able to carve.

All this sounds intimidating. It is merely a set of skills and terminology that need to be learned. Download demos, follow tutorials and it will make more sense. Ask questions. You'll get there.

Richard
 
1 - 12 of 12 Posts
This is an older thread, you may not receive a response, and could be reviving an old thread. Please consider creating a new thread.
Top