[Newbie] Using Cnc Cam To Drill?

[countryguy]

OK- Off to the next project. We're making a S45 type plasma machine torch holder. It will be Aluminum construction and should be another expansion of our CNC skills and learning.

I have the plate in the image below. I have two tasks on this plate. A) Get all the holes drilled and tapped. B) have the Mill cut the plate out from my larger stock piece.

Yet- I cannot seem to figure out how DolphinCAM can do the CAM initiated drilling for me. I simply wanted to let the CNC table make all the measurements and just drill out holes - Rather than myself going to do the squaring, layout marks, and drilling. I just assumed I would/could pop this on and let it go.

The drilling routine on dolphin seems to follow a "pattern" setup. (a grid or circle) ..anyway- I could mill out the holes as 'clears' and drill to size (was suggested) -

Maybe I am missing something here? Is this something you normally just do manually? Or have the DRO's just measure out and you then Mill-Drill.



TIA CG

 

[gr8legs]

I am not a Dolphin 'pro' - I bought it long ago with the hope it would do what I needed and it seems very powerful yet the user interface, the instruction manuals (hah!) and the customer support are all HORRIBLE.
With that said, here's an outline of how to get it to do what you want:
Place your drilled holes in the CAD system using the dimensions you desire - i.e. .250" for quarter inch holes, .375" for three eighths, et cetera.
Select all the features (holes, contours, etc.) you want to transfer to the CAM system.
The cad system will create a list of holes using the diameters you specified when you do: "Machining>Create NC> Patterns" and it uses the parameters you specified when you selected the hole sizes and depths. You can view these in the "Nc Gallery" which is the 'Nc" button (still in the CAD system). You can also edit depths here. The hole sizes you specified will be part of the 'PAT_XXX' where the XXX is the hole size you set.
If this looks sort of right then do Machining>Milling Module and this will start the CAM side of things and transfer your hole locations to the CAM side.
Now you are basically using the CAM system to help you write G-Code.
You first have to create a tool library (the button on the left above the M6 button) i.e. create your .250 and .375" drills, then select whichever you want to use first (using the M6 button), then the "Drill button (the third button below the M6 button) - then select which 'pattern' goes with that drill tool - which is going to be the group of drilled holes that are named Pat_XXX (as above).
Then change tools (M6 again) to another drill size and select the PAT_XXX that goes with that tool.
You can now try to view a simulation of your job. It may work or it may not.
Once you have the programming done then you need to post-process it for your cnc machine. That's the second button from the right on the top of the CAM screen. It may or may not work. With our Hurco machine the post-processing file Dolphin currently supplies is still wrong after we told them about it 10 years ago. I wish you the best of luck - you'll need it.
I am sure my explanation is more confusing than necessary - and that is (IMNSHO) because the Dolphin software user interface is not intuitive and their documentation is poor and the support is HORRIBLE.

 

[countryguy]

Thanks G8legs. I will experiment- I just wondered if the Drilling operations for parts were often setup and run thru CAM and the Mill? Or are is that type of work manually laid out and drilled on the corner drill press. To each is own I am sure. Dolphin just seemed lacking on the setup for drilling holes

Let me also ask the question this way- Is it normal to have your CAM software setup to do your drilling for you? I did setup two 'drill' tools in the library. I have the holes as 'contours' in the NC setup of CAD. I wondered if I should have put an X" mark though? Anyway- I think I'm moving pretty good thru Dolphin. I have a Q into Andre on CNC zone. Will post back when I get if all figured out.


Have a great day!
Jeff

 

[countryguy]

Dolphin noted I could simple have the Mill do area clears for the holes but that seemed a like a workaround? Since I need to thread them and attache stuff I was not sure if making a hole with end-mills and area clears would be good enough. Trying not to overthink this stuff- Just not sure what is the usual way to get a bunch of holes made via CAM. Yikes....

 

[RJSakowski]

OK- Off to the next project. We're making a S45 type plasma machine torch holder. It will be Aluminum construction and should be another expansion of our CNC skills and learning.

I have the plate in the image below. I have two tasks on this plate. A) Get all the holes drilled and tapped. B) have the Mill cut the plate out from my larger stock piece.

Yet- I cannot seem to figure out how DolphinCAM can do the CAM initiated drilling for me. I simply wanted to let the CNC table make all the measurements and just drill out holes - Rather than myself going to do the squaring, layout marks, and drilling. I just assumed I would/could pop this on and let it go.

The drilling routine on dolphin seems to follow a "pattern" setup. (a grid or circle) ..anyway- I could mill out the holes as 'clears' and drill to size (was suggested) -

Maybe I am missing something here? Is this something you normally just do manually? Or have the DRO's just measure out and you then Mill-Drill.

View attachment 111638

TIA CG

I'm still on my first cup of coffee and am not sure if this is what you are asking.

I use Mach 3 with SprutCam and there are a number of canned cycles for drilling and boring: G73: peck drilling; G80: cancel canned cycles; G81: drilling; G82: drilling with dwell; G83: peck drilling; G85: boring, no dwell, feed out; G86: boring, spindle stop, rapid out; G88: boring, spindle stop, manual out; and G89: boring, dwell, feed out. SprutCam gives me a variety of options for hole making and inserts the appropriate canned cycle in the G code.

For complex setups or where I have deep holes where I want to use peck drilling, I use SprutCam. For simpler projects, I will either use one of the wizards in Mach 3 or run manually. The advantage of running with the canned cycles is you eliminate the tedium of manually pecking, the reduce possibility of mis-entering coordinates, and reduce the machining time.

Bob

 

[gr8legs]

Dolphin noted I could simple have the Mill do area clears for the holes but that seemed a like a workaround?

As I said, support is HORRIBLE. This suggestion to mill holes instead of drilling is not your best option.
Do as I suggested in my first post: Lay our where you want holes and what sizes in CAD, transfer to CAM and let the CAM drill them. Drills are for drilling, milling cutters are for milling. Yes, many times you will mill out holes when you need to but most drilling is done with a drill bit, especially holes that are smaller or deeper than your smallest milling cutter..
With Dolphin you make that decision in the CAD side - if you select "Machining>Create NC > Contours" it outputs a milling operation, if you select "Machining>Create NC > Patterns" it outputs a set of points on your part to do an operation like Drilling. Selecting "Machining>Create NC > Both" is supposed to let you decide which operation to do where.
Once you transfer to the CAM side then you determine which tool does what operation.

 

[countryguy]

I have figured out how to setup my DolphinCAD/CAM for my drilling on a plate. The two JPG drawings show some info on what I did.
1) I imported my DXF of the plate with the holes center-marked. This could be as easy as putting a dot on your CAD or DXF. As long as you can select it, you can make it a drill point later.
2) Once the part is on the PartmasterCAD screen, I used a 'right-click' and selected 'Point Pattern' I usually am using the CAD product in 'contours' mode for Milling but in this case for Drilling Operations, the 'Point Pattern' is needed. See image below.
3) Remember to setup and use your "Group Numbers" to make it easy on yourself. In this case I make 4 point patterns. Pat_A1 thru A4. All group 0.
4) Save the CAD drawing and select "Milling Module".
5) When the CAM module loads you will see your point data on the screen. Start by selecting your drill tool.
6) From the CAM screen I used the 'drill' icon. From the small popupscreen you will see all your point-data you named and defined in PartmasterCAD.
7) I selected the label I gave my first spot. This was ' pat_A1' and insured the checkbox for machining all patterns with the same group number was checked.
8) Run the CAM scenario and Viola' The 4 holes are set to drill.

I am not sure if I need to make a new label at each point but will explore/experiment. This was really easy and the checkbox for working on items with the same group-id is a big time saver if you have not used this feature in other parts of the software.

 

[countryguy]

Bob- - Exactly---- Yeah, My Q was a mix of Dolphin but overall- I was not really sure that CNC and g-code had a set of "Drilling" codes for drilling type work. Your answer was spot-on about the general use of CAM for drilling. I get it now. Learned a TON in the past two days as we prep the next project.



I'm still on my first cup of coffee and am not sure if this is what you are asking.
I use Mach 3 with SprutCam and there are a number of canned cycles for drilling and boring: G73: peck drilling; G80: cancel canned cycles; G81: drilling; G82: drilling with dwell; G83: peck drilling; G85: boring, no dwell, feed out; G86: boring, spindle stop, rapid out; G88: boring, spindle stop, manual out; and G89: boring, dwell, feed out. SprutCam gives me a variety of options for hole making and inserts the appropriate canned cycle in the G code.

For complex setups or where I have deep holes where I want to use peck drilling, I use SprutCam. For simpler projects, I will either use one of the wizards in Mach 3 or run manually. The advantage of running with the canned cycles is you eliminate the tedium of manually pecking, the reduce possibility of mis-entering coordinates, and reduce the machining time.

Bob[/QUOTE]

 

[Bill C.]

I came into work one morning, years ago, this small shop bought a $150,000 CNC machining center, they were tapping 1/2" dia pins one at a time. They usually used a tapping head a drill press for such work. The tapping head was faster.

 

[derf]

I'd had 'um done on drill press by now.....
Why can't you just use manual data input?