The tutorial I find starts on page 3 and is missing the first two pages. I bit the bullet and jumped on the Dolphin band wagon versus the other guy and want to get a jump ahead with the demo while my program is in transit. I have milling down for pockets, goround, clear, and islands, but the drilling of holes is frustrating me. It only lets me go half way through the point drill pattern in CAD then screws up. Is this a demo problem, or I'm not doing something right?

Without making a point pattern, I can't do drilling in the CAM.

I know you have to demo so can't post files but can you be more specif in what you are doing ?
Have you drawn points or circles? are they on the same group ?

A picture of a sketch would be nice and we could talk you through it.

John S.

Actuually I figured it out. I was having problems with some functions disapearing,and my program locking up. Once past those hurdles I got the point patter to work, then got the drilling to work.

Found out there is a huge differerence between profile and contour when jumping into the DCAM.

I've managed to make tool paths, ramp in, spiral drill, center drill, peck drill face mill, contour, pocket with islands and contour with finish stock.

What I'd like to do is have the program go to the finish depth in layered steps for stock removal and can only do this by repeating a clear out over and over. I know for the pocket function there are stepped layers offered.but not it refuses poclket with an island and no layering in the clear out(?) option It could be my contour and profile poblems, but it is pretty easy ti pick up.

The hardest part is unlearning moves from other programs. Using shift to end a sequence versus shift to add to a sequence took some head scratching, then reading. Oh good golly I've been up all night with this. A new toy, a new game.

What I'd like to do is have the program go to the finish depth in layered steps for stock removal and can only do this by repeating a clear out over and over. I know for the pocket function there are stepped layers offered.but not it refuses poclket with an island and no layering in the clear out(?) option It could be my contour and profile poblems, but it is pretty easy ti pick up.



This one is easy.
In the Cad side you select your contour and it asks Z Surface which is normally 0.0 and Depth which for example we call call 0.500"

Now when you save and go into CAM it asks for a tool [ second icon down ] and you give it a diameter, again for example we will say 0.500"
Lead we ignore as it only applies to the pointy bit of drills, same for length as all that is the the graphical display of the tool [ don't know why it's there unless a visual to check you don't smack the vise with the spindle ? ]

Now the most important one Cut Depth, this is the depth the tool can cut per pass maximum, so we will set this at 0.125"

The result is now that the tool will machine the area clear in steps of 1/8" per pass, doing 4 passes until it reaches 0.500"

John S

This one is easy.
In the Cad side you select your contour and it asks Z Surface which is normally 0.0 and Depth which for example we call call 0.500"

Now when you save and go into CAM it asks for a tool [ second icon down ] and you give it a diameter, again for example we will say 0.500"
Lead we ignore as it only applies to the pointy bit of drills, same for length as all that is the the graphical display of the tool [ don't know why it's there unless a visual to check you don't smack the vise with the spindle ? ]

Now the most important one Cut Depth, this is the depth the tool can cut per pass maximum, so we will set this at 0.125"

The result is now that the tool will machine the area clear in steps of 1/8" per pass, doing 4 passes until it reaches 0.500"

John S


I found another way to do this. When you select the contour to be machined, you can set the depth of the contour, but if you go to the tab labeled Z (feed?) you can put the maximnum cut depth down and override your tool's maximum depth. So for one operation you can use all of the endmill's cutter length, but if you want to step pocket, setting a Z cut limit will use the tool as if it were originally set up with a shallow cut profile.

Pretty interesting, they really need a manual a person can read at will and have at their side so the you can work and read or look up a problem as you go.

Sometimes my demo hangs up for no apperent reason. I found if I go through a tutoirial and use the DCAM from the tutorial, it is less glitchy for some odd reason. I'll be watching my mailbox daily for the package now that I'm getting the hang of it. I want to make chips!

Mr Wild,

We can get you activated before your package gets there. That is no problem. Secondly, the reason we do not actually ship out a hard copy manual is simple. It would raise overall costs for the end user due to printing, putting together, shipping etc...
Some customers pay for the manual upon request. Most think it's better to print the manual from the CD. (Save costs)

Hope this helps.

I found another way to do this. When you select the contour to be machined, you can set the depth of the contour, but if you go to the tab labeled Z (feed?) you can put the maximnum cut depth down and override your tool's maximum depth. So for one operation you can use all of the endmill's cutter length, but if you want to step pocket, setting a Z cut limit will use the tool as if it were originally set up with a shallow cut profile.



Interesting.
Like a lot of machining there is never a right and wrong way to do things, just different ways.

I use the way I posted because setting the cut length in the tool setting forces it to cut to this depth in every process that uses this cutter.
So if you have a small cutter say 1/8" that's limited to say 1/16" max depth in steel without breaking [ just figures ] then you have to purposely over ride this if you need to instead of having to reduce the depth.

Not saying my way is the best as I'm self taught anyway it's just another way.

Just as an example if I were doing an area clear that had to look nice as opposed to just blocking out metal I would set my tool to a cut depth that was suitable for the material and then in area clear, or goround, same method,
I would select the contour and apply say 0.010" in the XY and Z boxes for a clean up pass.
I would then do a second area clear or goround, same contour but leave the xy and z boxes at zero this time and then swap to the options tab.
Under options I would then click 'ignore cut depth setting for current tool'

What happens then is the tool does the process in step depths as applied in the tool selection leaving 10 thou on all round and then it does a final pass at full depth removing the last 10 thou to leave a nice clean up pass.

One other option to note is the one above this one called ' Machine all contours with the same group number'
This really needs to be in a thread of it's own, feel free to start one, but heres a quick run down.

In CAD when you select an contour at the bottom you have a group number, they are a lot like CNC versions of layers.
If say you have four pockets round a central boss you select them and name them, say pocket1, pocket2 etc and give them the same group number, again say 2
Do not put anything else on group 2.

Then in CAM select the operation, say area clear, select pocket 1 and tick ' Machine all contours with the same group number'
What happens then is the tool machines pocket1 then pocket2 etc without having to define 4 operations.

Note though that all pockets have to be at the same depth as pocket 1 as it uses the same information through all processes.

It often means you can have a very bare program operations list but it does a lot of work

John S.

i find a bit of forethought in the cad side saves loads in the cam side
using the group feature being a big help
the other thing is to offset areas so you can do an area clear and over clear the area
ie a square block offset by say 5 mm ,if your first cut is a go round followed by an area clear it will leave an uncut area the offest will ensure this wont happen
you can still have an island in this unlike face mill option
partial machining is a good one too
means you can machine a part on a piece of stock then effectivley part it off if you
cad an area that is cleared to part the piece off
mike