[lgalla]

HI GUYS,
I have been on the forum for months designing a 6'X12' router.I must say thanks for all the help,I am sure I can build the machine.My weakness is software.I build speaker cabinets which is rabits ,dadoes,circles etc.Pretty simple stuff I imagine.What would be the easist,simple CAD/CAM to learn.I have tried intelicad and other free demos but I just fight with them.I tried E-machine shop and it is friendly and learable but of no use for your own machine.Friends have software like solidworks which is beyond my learning capibilities and I don't have a spare $20,000 grand.I just E-mailed Dolphin CAD/CAM to ask these questions.When you are older[55]and have limited computer skills,it is very difficult "to teach old dogs new tricks"Any suggestions as to a starting point or software so easy my dog could do it.
Thanks
Larry:violin: :drowning:

[ger21]

Look at DesignCAD and SheetCAM.

http://www.imsisoft.com/prodinfo.asp?t=1&mcid=398
www.sheetcam.com

[lgalla]

WOW
Dolphin already responded while I was posting.They have people working late and said to call.A bit fast for me before hearing from the Zoners.I request some help or info before responding to them.
Thanks
Larry

[lgalla]

Geof
R/U/Following me?I can't seem to get away from your chair thing.(chair) (chair) (chair) (chair) (chair) (chair) (chair) (chair) (chair) .Maybe you can drive some sence into my head.Your expertice is highly regarded.:cheers: :cheers: :cheers: :cheers:
Larry

[Geof]

Geof
R/U/Following me?I can't seem to get away from your chair thing.(chair) (chair) (chair) (chair) (chair) (chair) (chair) (chair) (chair) .Maybe you can drive some sence into my head.Your expertice is highly regarded.:cheers: :cheers: :cheers: :cheers:
Larry

Calm down I don't type fast!!

I will probably get all the CAD/CAM people jumping on me for this. If you are doing straight lines and circles probably the fastest way to get into making things is learn G code. It is not that difficult I taught myself G code programming on a lathe in '99 and I was an older dog then than you are now.

I know some people treat G code as if it was some arcane secret, understandable only by the initiated few but it is really fairly simple. There are two basic modes in which G code operates; incremental and absolute. When you are using incremental all the code is doing is telling the machine 'move this distance in this direction'.

G91 says make this move incremental
G01 says make this a feed move at the specified rate
X30.0 says move 30.0 units (inches or millimeters) along the X axis only
F10.0 says move at the rate of 10.0 units per minute

The full command is expressed in a block;

G91 G01 X30.0 F10.0

Some commands persist; they are 'modal' commands and the next block could simply say;

Y20.0

Because the G91, G01 and F are all modal this move will be a distance of 20.0units along the Y axis at the rate of 10.0 units per minute.

I compare incremental to reading the proverbial pirates treasure map; so many paces north, so many east, etc.

The other operating mode is absolute and I compare this to map reading. You could, with a bit of difficulty maybe, go from wherever you are now directly in a straight line to Portage and Main in Winnipeg. That is an absolute command; go from where you are now to a specific destination.

In absolute mode the destination is the important point not the starting point and you need a way of defining destinations. This brings in the idea of the 'Machine Coordinate System' and Work Coordinates. The machine coordinate system is based on a constant location somewhere on the machine. On metalworking machines convention places it in the far right corner compared to the operator's normal position with the tool raised as far as possible above the work table. Wood working machines may use a different convention. Once you have this reference location called Machine Home or Machine Zero you could specify every point that the tool can reach by three numbers; the X, Y and Z coordinates. But this can be very awkward so a secondary reference point is used called a Work Coordinate or Work Zero or Work Offset. You can place this Work Zero wherever you want within the range of movement of the machine. For example if you want to cut a circular groove in the center of a panel you can make the location of the center of the circle the Work Offset.

Using Handle Jog you move the machine until the tool is centered on the location of the circle and is exactly at the surface of the workpiece. The machine knows where this is either by encoder feedback or because you have stepped a certain distance on the three axes. So you know the coordinates of this location; they are displayed on a screen somewhere. These coordinates, the X, Y and Z values are entered into an 'Offset Table' under the identity G54.

Continuing with the example; your groove has to be 1/2" wide, 1/2" deep with the inner side of the groove on a 10" diameter circle. You can use a 1/2" diameter bit and that settles the width of the groove.

First you tell the machine to move to the center of the circle using the following black of instructions;

G54 G00 X0. Y0. Z1.
This tells the machine 'Go to the location specified by the coordinates in the G54 entry in the offset table and stop zero distance away in X and Y and +1", i.e. 1 inch above in Z.

Now you go to a point on the circle so that the inner edge of the cutter is at a 5" radius and is just above the surface;

X0. Y5.25 Z0.1
You have moved the center of the cutter 5.25" so the inner edge of the cutter is at a radius of 5" and it is 0.1" above the surface.

Now move the cutter down to the groove depth. (Of course in real life you would have turned on the spindle but don't worry about that yet)

G01 Z-0.5 F10.0
Using a feed motion the cutter has cut its way to the depth of the groove.(This actually is not the best way but is good enough for an example)

Now cut the circle.

G03 I0.0 J-5.25
G03 says to the machine go in a circle around a center point located -5.25" away on the Y axis and come all the way around back to the starting point. I refers to X distances and J refers to Y; you only moved Y from the center of the circle to your starting point for the cut.

Your groove is done now lift the tool clear.

G00 Z1.0

The job is finished now tell the machine to get out of the way so you can take the part off.

G28
This is just a short hand which says 'Go to machne home on all axes'.

Needless to say I have omitted stuff such as what speed to run the cutter and starting and stopping the spindle. Also it is obvious that if you wanted to use two tools they would both have to be exactly the same length if you used G54 to specify X, Y and Z. Different tool lengths are handled by having a Tool Offset which is just a Z coordinate for a particular tool entered into a Tool Length Offset Table. Then an additional command is used: G43 H01 which says to the machine use the value in the Tool 1 entry in the Tool Length Offset Table.

Taken all at once G codes can swamp you. They have no intuitive meaning just arbitrarily assigned functions which does not lend itself to easy memorizing. Taken bit by bit they are simple; a bit like learning line dancing but without a caller.

The other side of programming, the M codes are the same; arbitrary meanings such as; M03 Start Spindle Clockwise, M05 Stop Spindle. But these also can be taken bit by bit.


And don't expect a reply to any questions until after Feb 28. I am going on vacation far enough away to be out of email contact.

[ImanCarrot]

Personaly I like AutoCAD (I beleive you can get AutoCAD Lite fairly cheaply), to the point that I export my drawings into Dolphin to post process it into G Code... I simply cannot get the hang of Dolphin CAD (not dissing it, it's probably just me).