Ramped lead ins

[hwd_woodworking]

I was talking with a friend that works with a big CNC and he pointed out that the larger ones will lead in to most cuts. That is lead in from the surface and by the time it arrives at the profile it is at the appropriate depth. I was wondering if any one has played around with this.

When we cut our melamine we use a 1/2" compression bit and we normally just plunge right at the profile. As soon as the "downcut" part of the bit enters the material you no longer have good chip evacuation. Our stock is mostly 3/4" and by the time it reaches the full depth it has heated up considerably (sometimes slightly burning). I believe this causes my bit life to shorten. We use part Wizard 2 and don't have the option of peck drilling. So this thought about a plunging lead in got me wondering if it is even worth trying.

[gerald_d]

Hi Nathan, you might want to peruse or pursue this thread. (http://www.talkshopbot.com/forum/messages/1038/1095.html)

[paco]

Hi Nathan!

It would sure be worth trying and I'm quite positive that it would help you but you wont be able to programed this automatic in any way with PW2; you would need more options from your CAD/CAM...
One thing that I can think of as a work around until you can have more options would be to "drill" a hole larger than your tool bit diameter just about the lead in begining in PW2 and then start your cut from this hole... this drilling could be done in several pass and about 1.25-1.5 your tool bit diameter... this would leave room for chip extraction but will sure take more of your time to machine a whole sheet...
Hope this help...

[elcruisr]

You are correct that a ramped lead in will extend tool life. One of many reasons we upgraded our software. We now do 10 degree ramped and curved lead ins. Better tooling life and part quality are the result.

Eric

[ron brown]

Ramps can be written in "by hand".

Ron

[wayne_walker]

I have been using a ramped lead in to do the clean up on a 1 1/4" hole in ABS plastic. I just purchased a single flute up spiral bit from Onsrud Cutter and they recommend a spiral plunge but I can't figure out how to set it up in PW2.

Any help would be appricated. Thanks in advance.

Wayne

[Brady Watson]

Wayne,
You cannot do a ramped XZ or YZ move in PW...but you can do something like this:


5158

If this is a clean-up pass then disregard the small circle in the center, since the center hole will be clear. Do an inside profile in PW and select 'Add Lead-in'. I have chosen a circular one in this example. If the center circle is not clear, then drill a 1/4" hole (might want to do one a little larger) and run the profile/cleanup toolpath on it with the lead in. (toolpath lead-in profile pass 1st...then sketch drill hole in so you know where it is) You should be able to drill all of your holes and then just use your single flute bit to profile and finish in one shot by starting in the drilled hole.

Does that help?
-Brady

[ron brown]

Wayne,

I will sometimes use Rhino to make "interesting" plunges, exits and tabs. Since I have Vector, the odd moves and control of bit are not a problem. If the plunge can be kept in the same location you might draw and path your DXF to SBP converter and manually insert that file in your code.

Ron

[wayne_walker]

Brady and Ron,

Thanks for the quick responce. As a new user, the only software I can use at the time is PW2. I have AUTOCAD 2000, but I have just begun to learn how to use it. The part is drawn and pathed in PW2.

I have 400 parts to cut with 3 holes in each one. I am cutting 32 parts at a time. I do not have a second Z, can I drill the hole with the single flute bit by just controlling the plunge rate?

I am using the PC router so I am limited to the 5 speeds on the machine. I have a PR up upgraded to a PRT.

Thanks Again,
Wayne

[Brady Watson]

Wayne,
The reaason that you are doing the drilling is to get around the fact that single flute tools don't plunge straight down very well.

The easiest way for you to set this up is to toolpath one part, draw the drilling circle where the lead-in falls and then delete the toolpath. Then block-copy the parts to create rows and columns of parts. Group all of the big circles as one part and all of the small circles. Then calculate the drilling toolpath (for all drill holes) and then all of the profile passes with lead-ins. Preview both of the toolpaths in the Windows software previewer (even if you are not running it on your tool). Run both of them consecutively and make sure that the drill and lead-ins match up...which they should.

In regards to drilling with the single-flute bit...don't. Go buy a cheap 1/4" bit from the hardware store or use a 1/4" drill bit to drill the holes. Since the holes will reside in the scrap, it doesn't matter what you use to drill...You probably *could* use the single fluter...but it's not worth breaking for drilling.

-Brady

[gerald_d]

Wayne, what size bit are you planning to use? We have no problems plunging a 1/4" single flute Spiral-O Belin bit straight in. For most work we use 2-flute spiral "slot drills" that are designed for both drilling and side-cutting.

ETA: Cross-post with Brady

[wayne_walker]

Brady and Gerald,

I am using a 3/8" bit.

I figure that they were not designed to plunge, I just need someone to tell me that, to save the $30 I just spent on the bit.

I have not done a bit change in the middle of running a program before but it is time I did!

This is the first real project, the other material I cut was more or less just learning to use the machine.

Thanks
Wayne

[mikejohn]

Wayne
In AutoCad 2000 it really is simple (PW defeated me because I could not tell the program to cut in a particular order, but Im not a PW user).
I drew this in Autocad.
5159, then I converted the .dfx to .SBP, went into an editor and simply raised the start of each line 1mm in turn. (I took a cutting depth of 5mm.

The file then looks like this

J3,4.2828,17.0958,0.0000
M3,2.9979,9.5356,-1.0000
M3,6.1388,3.9725,-2.0000
M3,13.1346,1.1196,-3.0000
M3,21.2725,4.2578,-4.0000
M3,24.9845,9.9635,-5.0000
M3,26.0000,13.0000,-5.0000
CG,,26.0000,13.0000,-13.0000,0.0000,,-1

Not a true spiral I know, but you do get closer to your circle cutting line after each line, and you finish by coming onto the circle at the correct depth, at a narrow angle to the circle,
All achieved with no bit changes.
The shopbot simulation looks like this.

5160

..............Mike

[bill.young]

Wayne,

If the holes are laid out in a regular array on the sheet you could use the Drill Press Virtual Tool (TD) to create a file to drill a sheet's worth of holes...spiral plunge is one of it's options.

Bill

[wayne_walker]

Mike and Bill,

Thanks for the input.

The holes are not on a in a regular pattern. So I used Mike's suggestion.

I waded thru Autocad and made the semi-spiral leadin. After pulling my hair out and with the help of Frank at Shopbot, I figured out the tool path. It spirals down and does the profile like it should.

Mike, how do I make a block copy with this hand built spiral?

Thanks for any help.

Wayne

[mikejohn]

Wayne
Is there any regularity in the position of the pieces?
The Aray command allows you to select any number of objects (here the 'spiral'and circle) and create any number of rows and columns.
If the circles are randomly scattered over the worksheet,and you wish to place the end of the spiral at a particular position on the circle, then 'remove' a very small piece of the circle, say0.001", join the ends together with a line,
Right click on OSNAP at the bottom of the screen and deselect everything apart from the first choice Endpoint.Select OK
Make sure OSNAP is on.
This time we move the ends differently. Starting with the 'spiral' line that touches the circle, double click on it. This brings up the properties box. (If it doesn't, click on modify then Properties from the menus.) The end of the line should have the same Z as the circle. Change the start of the line Z by 'lifting' it the required height. Now go backwards line by line, lifting the end to the previous lines Z start height, and lifting the Start of this line to the desired new height.
When you have completed all the lines, select COPY, and copy the 'spiral' lines. When asked for Specific base point or displacement, or [Multiple]: type m. Now choose the end of the line that will join the circle and select. Now go from circle to circle, clicking on the very short line you created.
Now you have all the 'spiral' lines in the correct position.

There are more ways of doing this, but without more knowledge of how your sheet is laid out, I can not offer more assistance.

If this isn't clear, come back again.

.............Mike

[mikejohn]

Wayne
You 'remove' a piece of the circle by crossing it at the point you wish with a line, offsetting that line 0.001" then trimming the piece of the circle between the lines.
Zoom way way in for this

...........Mike

[wayne_walker]

Mike,

I have sent you the art and cut file to review. I think I have the spiral set up correctly. I don't know how to get the spiral tool path to the remaining parts without modifing each one.

Thanks again for your help.

Wayne

[gerald_d]

Mike & Wayne

I would only build one spiral lead-in plus complete circle as per Mike's method, but I would do it on a different layer to the original circles. Then I would use the Multiple Copy (as Mike described) to copy the fancy circles to all the old circle positions, switch off new circle layer, delete old circles, switch new circle layer back on. This way means that you find the tiny break only once and saves you from trying to find many tiny snap points.

In summary, the answer to Wayne's "how do I make a block copy with this hand built spiral?" question, is to use the Multiple Copy method instead of Block Copy.

(Mike, remember that Wayne is limited to 2D in PW, so it doesn't help him to fiddle with the z heights in AutoCad. I think that he is only trying to do the "flat" spirals.)

[wayne_walker]

Mike & Gerald

I have run the spiral and hole profile of the first part, which has 3 holes in it, on the Bot and it worked fine. I need to work out the feed rate and RPM. Is it possible to copy the tool path from one part to the next?

When I delete the tool path to reveal the line of the spiral below the tool path (machine along vector path) it deletes the line of the spiral which I imported from AutoCAD.

When I block copied the part, it copied the part with the 3 holes but not the imported spiral from AutoCAD.

Thanks, Any help is appreciated.

Wayne

[gerald_d]

Wayne, if you are talking about the stuff that you need to do in PartsWizard, then Mike and I cannot help you - we use different software to go from the AutoCad dxf to the ShopBot sbp.

Can the PartsWizard guys offer Wayne some help?

[gerald_d]

Mike, are you guys okay in the floods?

[Brady Watson]

Wayne,
Don't delete the toolpath...just turn it off by unchecking the box for 2D.


5161

You have 2 options for setting up multiple copies. 1st you could get one set completely toolpathed and use the S_Nest.sbp file in SBParts to do a sort of toolpath block copy using the Windows software. 2nd, you could align the imported DXF with your other geometry, block copy it in PW, group it and toolpath it. Then repeat for the other parts. Everything should line up exactly.

-Brady

[ckurak]

There is another way to get an entrance cut with PW: Use the "Plasma Lead In" on PROFILE cuts. It is NOT a ramp, but does plunge the bit into the material away from the final workpiece.

Charles

[Brady Watson]

Zactly Charles...that's what I posted above...but didn't indicate that it was a 'Plasma' lead in.

-Brady

[wayne_walker]

Brady and Charles,

Thanks for the help. I have been having computer hardware problems over the last couple of days. So, I have been directing my attention to that issue right now.

Once I get the hardware up and running, I'm sure I will have more questions.

Thanks,

Wayne

[mikejohn]

Charles and Brady
If all you wish to do is plunge to the required depth somewhere in the centre of the circle, then move to the start of the circling cutting, wouldn't a simple MZ command work?
.............Mike

[mikejohn]

I just drew a circle in part wizard, created the toolpath and saved the.sbp to illustrate the above.
When I opened the file, instead of a CG command I found a large number of M3 commands instead.
Anyone tell me why?
....................Mike

[mikejohn]

Actually ticking lead in does the same thing, or am I missing something?
.............Mike

[gerald_d]

Mike, it drives me nuts to receive .sbp files from SB'ers that have been created in PW. Instead of a single CG command for an arc, there is a whole row of M3's and CG's breaking the arcs into tiny segments. This makes it impossible to find the exact center of the original arc.

There are two different concepts being mixed up in this thread......
- A certain style of bit that cannot drill, or be plunged straight into the job. This bit needs to be "ramped" down an incline - it needs to move horizontally as well as vertically when it enters the material.
- A tangential lead-in to the finished profile so that you don't see a burn mark (etc.) where the bit plunged in. This is the "plasma" thing. This is not going to make a non-plunging bit willing to take the dive.

[Brady Watson]

There are no CG commands in the Shopbot_Inch post. You have to choose the Arcs_Inch post.

If Wayne can just do an 'MZ' then we all just wasted a bunch of time telling him how to do a lead-in...

-Brady

Cross-post with Gerald...and clarification:

The whole idea here is to compensate for the fact that you cannot do a ramped lead-in with PartWizard. BUT as I have illustrated above, you CAN dril a hole where a plasma lead-in begins to allow the bit to drop into the hole on a profile pass (using the plasma lead in and regular arcs_inch post) to acomplish the same basic function as the ramped lead-in.

Is it more work? Yes. Does it require you to rack your brain as a new Shopbot user...maybe a little, but nothing unreasonable. Do you have to do a tool-change from a drill bit/2-fluter to your expensive bit? Yes. Big deal.

[gerald_d]

I don't like the idea that a software limitation forces a tool change.

[mikejohn]

Just so I fully understand.
The ShopBot command for arcs (circles are special arcs) is CG.
The CADCAM software supplied with the ShopBot (PW) doesnt recognise this command.
...............Mike

[gerald_d]

Mike, here is a an example of a single circle (after the first M3 line) in sbp code from a SB'er with PW:

M3,16.735161,2.443232,-0.37500
CG, ,16.755024,2.466739,0.189136,-0.385899,T,1
M3,16.755024,2.466739,-0.375000
CG, ,16.818228,2.458557,-0.023341,-0.428530,T,1
M3,16.878308,2.441337,-0.375000
CG, ,17.099515,2.262374,-0.153544,-0.415980,T,1
CG, ,16.975413,1.641192,-0.385619,-0.245947,T,1
M3,16.920377,1.608793,-0.375000
CG, ,16.541454,1.608793,-0.189461,0.386766,T,1
M3,16.486418,1.641192,-0.375000
CG, ,16.325116,1.841603,0.257348,0.372247,T,1
CG, ,16.486418,2.391178,0.422642,0.174412,T,1
M3,16.541454,2.423577,-0.375000
CG, ,16.755024,2.466739,0.189136,-0.385899,T,1

So, it seems that PW does generate CG commands. But a single line of CG code would have been enough to do the full circle.

[benchmark]

I found a simple way to write a spiral plunge in Shopbot code is to use the Drill Press function in the Virtual tool....Decide where you want the hole, when you tick the "use pocketing for thru-hole" it will write the code for a spiral plunge.... which I then paste into my cut file.



Paul

[bill.young]

Hey,

Here's a simplified version of another option. The variables &center_x and &center_y below are the center points of the circles...you could add as many points as you wanted. It may not the most efficient way to do it if you have 100's of holes but gives you a nice spiral plunge. This version does a spiral plunge with a bottom cleanup pass (the 4 at the end of the CP command), but there are lots of other options for the CP command that you can find out about in the help file.

To try it out just copy the section below and paste it into a blank ShopBot file (typing FN gets you a blank ShopBot file in the software). Save it and then run it in preview mode and you'll see the spiral plunges.

Bill

'********************************************** **

' These three lines define the center point
' and call the circle subroutine. Repeat them
' for each circle that you need, changing the
' values of &center_x and &center_y.

&center_x = 2
&center_y = 5
GOSUB drillcircle

&center_x = 6
&center_y = 10
GOSUB drillcircle

&center_x = 17
&center_y = 5
GOSUB drillcircle

END

drillcircle:

[mikejohn]

Bill
One thing I am learning is the power of the ShopBot language, when either writing direct commands or editing converted files, to get what you want.
The circle command was defeating me a bit, but I am slowly getting the hang of it.
..........Mike

[bill.young]

Hey Mike,

The CP command is the most logical for me...it uses the center point to define the location of the circle. The CC command is great if you want to do an arc or circle using your current position as the start point...that's the one that I use to create my wavy scarfs because all I need to know is the size of the waves and which way the waves are headed.

I've never been able to make heads or tails of the CG command, so I don't tend to use it.

Bill

[mikejohn]

Ah!
So I'm not the only one having confusion with CG.
Time to look at CP!
...........Mike