cnc procedures

[mike hide]

this is a bit longwinded, I have built Joes 2006 machine with minor mods ,built the hobbycnc 4 axis system and subscribed to Mach3 and Sheetcam.Everything seems to be working.

Now I am desperately in need of cnc procedures using the software described.As a trial I produced a CAD drawing of a corner fret[excuse the drawing I am new to CAD also].The drawing consists of several layers,basically just to experiment with [some will be on the same depth].

I have followed the two tutorials in sheetcam and am not sure if the pocketing one would automaticall cover all aspects of the profile tutorial of if it is necessary to do both. I have no idea how to approach the holes .Looking at parts cut by Joe for his machine to produce a radiused corner the bit goes past the vertices or will the bit only drive so that the corner ends up with a radius the same as the bit radius ?

Any help appreciated or perhaps suggestions for suitable tutorials...regards mjh

[ger21]

First, you need to work on your CAD skills a bit to get a cleaner drawing to work with. Once that's squared away, here's how I would do it. Example pics from V-Carve Pro. I also attached a clean drawing with the appropriate layers to do what I did.

Create a square to remove all the material at the depth of the highest part, in this case the straight 1/4" wide straight pieces on the side and top. I called this layer Bracket.

Create another square to cut down to the depth of the first scroll, inside the frame that we cut on the previous layer. I called this layer Scroll Face.

Create another layer for the first scroll. The scroll will be an island inside another square, because we're removing the material around the scroll. This layer is Scroll 1.

Create another layer for the second scroll. Since you don't want to cut away the first scroll, this layer is a combination of both scrolls. The previous layer cut to the face of the second scroll, which this layer will pocket around. This Layer is Scroll 2.

Create another layer for the square holes. You can either cut the perimeter of the holes, or pocket them. I pocketed them in the pic to make them more visible. This Layer is Square Holes

Finally, Create a layer with the perimeter of the object on it, to cut out from your stock. I called this Perimeter.

I let V-Carve offset all the toolpaths, so they cut to the lines rather than along them. You'll have to have SheetCAM offset them as well. Another option is to do the offsets in the drawing, but if SheetCAM will do them, it's easier to do it there.

For specific SheetCAM questions, ask either in the SheetCAM section here, or on the SheetCAM forum. Les should get you going pretty quick.

[mike hide]

First of all thank you for your timely response . I do not have "v carve", not affordable in my case. But I will try and work through your procedure and insight with the software I have .

When I try and open the cleaned CAD drawing I get this window saying

"M3 plugin installed-plugin installed" is there a way to get rid of this so I can see the drawing ?

[ger21]

Mike, I don't have SheetCAM, but the process should be the same. I just used V-Carve to give you some pics to see what i was talking about.

What are you trying to open the drawing in? It's just a basic .dxf.

[mike hide]

I HAVE "TURBOCAD 6.5" which seems to work fine .I don't know but any DXF drawings I have on my computer seem to suffer the same fate .I try and open them and the window with M3 plugin installed appears but no drawings.That includes DXF drawings made on my own computer in turbocad.Furthermore I cannot seem to find any M# plugin anywher on my computer. Might it be some kind of virus?

[ger21]

Sounds like the .dxf extension got assigned to the Mach3 plugin file type. You can always start TurboCAD and then open the .dxf from there. You should only see the error when double clicking on them. You can also try right clicking on them and choose "Open With" if that option is available.

You can also try correcting it by going to My Computer, choosing Tools > Folder Options, then file types. Find .dxf and see if you can re assign it to TurboCAD.

[mike hide]

Ger.I am still in a quandry.Sheetcam requires one to declare the toolpath, inside the line ,outside or on the line . and also define the layer .

The scroll 2 and scrollface layers ,as I see it would require the tool paths to run on the outside of the scroll but on the inside of the perifery..help again please

[locost_cam]

Hi Mike,

First of all, you need to be careful with your drawings. Lines must join up exactly. You cannot have any gaps or overlaps. Remember the machine has to follow the outline smoothly. A gap would be machined as a gap, which is not what you want.

When you load your drawing into SheetCam you will see that some of the contours are colored red or yellow and some are grey. The grey contours are broken - i.e they have a gap or overlap. Go to View->layer tool and turn off all layers apart from one. Make sure view->show segment ends is turned off and view->show path ends is turned on. This puts a little white dot wherever lines don't join up correctly. If you zoom in closely you will see the problems. In each case you need to go back to your drawing and correct them. This is a slow and sometimes irritating job but I am afraid it has to be done.

A note when drawing, get used to snaps. They are your primary weapon against alignment problems. When drawing, wherever possible use a grid snap. this will force any points you place to be on the nearest grid intersection. Set up your grid to a fairly small size. After grid snap, end point snaps will put your point exactly on top of the nearest existing point on your drawing. Once you get used to snaps you will wonder how you could work without them. Also investigate the trimming functions available in your cad. Most packages have functions to automatically join two lines/arcs exactly.

Your drawing is quite complicated and I'm not too clear what you want to achieve. I have attached an example job using Ger's cleaned up drawing. It cuts a similar design to Ger's example. I used metric because that is what I am used to. However the numbers don't really matter at this stage.

Like Ger I first cut the BRACKET layer to recess the area where the scrolls will be. For this I used a spiral pocket 2mm deep. You could save quite a bit of machining time if you cut off the unused corner of the square. At the moment you are machining away a lot of material that you don't need to.

Next I did a spiral pocket on layer SCROLL_1. This leaves the upper scroll higher than the rest.

Next comes the second scroll. Using Ger's drawing everything surrounding the two scrolls is machined to a depth of 5mm.

After that we need to cut the shape out. I tweaked the drawing in SheetCam and put the squares on the perimeter layer. I did an outside offset because I want to cut the shape out of the sheet. SheetCam works out that the squares are inside the perimeter so it cuts inside them. Inside contours are always cut before outside contours. In SheetCam outside contours are red and inside contours are yellow. You could cut the squares separately but this way saves time and effort.

The resultant part has the upper scroll machined 2mm deep, the lower scroll 4mm deep, the area around the squares 5mm deep then the whole thing machined 10mm deep, using 10mm material.

Note the attached job is zipped because the forum won't accept SheetCam job files. You need to unzip the file first.

[locost_cam]

Originally Posted by mike hide Looking at parts cut by Joe for his machine to produce a radiused corner the bit goes past the vertices or will the bit only drive so that the corner ends up with a radius the same as the bit radius?

SheetCam will try to cut what you draw as closely as possible, within the physical limits of the machine and cutter. if you have a sharp inside corner you will end up with a radius equal to the cutter radius. If you have an inside corner with a radius greater than the cutter radius then the resultant radius will be as drawn.

If you need to create a recess for a sharp cornered part, SheetCam has an option in the 'cut path' tab called 'overcut corners'. This will cut into sharp inside corners to allow a sharp cornered part to fit.