Toolpath from the side

[kubotaman]

I am currently learning about using the indexer and I have a question. Magnate makes extra long bits that cut better from the side than say the same comperable cut from the top using the indexer. How would one create a toolpath that makes this possible, especially if the bit has to follow in and out of a turning made on the indexer? A straight cut I can understand but a non straight cut has me confused. Hope I have made my question clear. I have no drawings. I am just thinking how it could be done. Thanks!

[ssflyer]

Hi Daryl,

Not sure about the indexer - i've only got my stepper and lathe for my home-built, so far, but almost all bits are made to cut from the side. I may not be understanding the question, but it isn't really different from cutting a flat surface, since the indexer should simply move your router/spindle in the Z axis...

[myxpykalix]

Daryl,
What you are looking at are bits like "side reeding or fluting" bits and that is meant only for straight indexed toolpaths around a circumference not to be used with a toolpath that spins the indexer but only rotates it to allow a series of passes around the outside.

[kubotaman]

Jack your picture is correct. But my question is how would a person make a file to go in and out of the "valleys" like your picture shows in the leg drawings. I realize that the bits are not to be cut while the indexer turns, they are to be used in forward cuts only, X axis only. I am just curious how to bring in the bit from the side to cut high and lows of a turning.

[dana_swift]

Daryl- I understand exactly what you are asking for. If you use Aspire to create your toolpaths, you can create a custom post processor that uses Y (or X) instead of Z. The machine will not know the difference. For safe Z you will have to retract Y to the same safe distance that Z would have to retract in a conventional setup. This is all easy to do with a custom post processor.

The custom post processor must set Z to a depth such that the side of the bit is exposed to the centerline of the indexer within the "cutting edge length".

For your bit definition you must use a "ball nose" with the radius of the tool. Then you will get the toolpath you need. As with any ball nose it cant get into the V's in Jacks drawing any different than a ball nose in conventional cutting.

Make air cuts until you are sure the post processor is running correctly, then go for it!

I have not cut anything in that mode, but had already thought out how to do it, I think it should have some distinct advantages over "Z" indexer cutting. Good luck, and keep us posted!

Hope that helps-

D

[kubotaman]

Dana, you and I understand what I am after. There are advantages to what I am asking for. I also realize that it can't get in the valleys just as from the top. A bit cutting from the side will definitely be a cleaner cut than from the top. The center of the bit cutting from the top really isn't cutting where as from the side it is. The advantage is a much cleaner cut. I understand what you are saying. Where can I get the info on making a "custom" post processor. Can I ask questions to you if possible? Thanks for the answer.

[myxpykalix]

Daryl,
I know what you want to do. Your profile of the part is part of your toolpath.

You would make a toolpath just like if you were carving this design in a flat piece. see pic
You would go to the centerline of your indexer then Zero your Z.

make the toolpath according to the picture

run the toolpath once

Do a MB 10 (to rotate the indexer 10 degrees or whatever you choose)
Repeat till you have an equal number around 360

As far as doing it within a particular program wizard, i can't tell you. I don't know if this makes it any clearer or not, not sure if i explained it correctly.

[steve]

hi Dayrl, I have used the cutting from the side method with those long bit from Magnate. To creat the toolpath I use part of the vector used to create the item. i have to pay close attention, the Y axis really acts as the Z axis ( as was mentioned by others) . I think you've already figuared that out, anyway here is a picture of toolpath vector created in Artcam.
Also a link to another post I did this way.
http://www.talkshopbot.com/forum/showthread.php?t=10837

[kubotaman]

I understand what everyone is saying. I also understand that the Y axis has to act as the Z axis. My question is how does one go about it? Is a "custom" processor the answer and if so where do I learn how to make the processor?

[myxpykalix]

Daryl,
You don't need to make a post processor but simply a toolpath. Stepen's post above and the link he cites shows more concisely what i was trying to draw out clumsily.

What i think you want to know is, once you draw out the vectors how do you make the toolpath so that it travels in the vector path you make then controls the indexer and rotates it and repeats the pattern. Am I correct?

I can do it manually like i explained earlier and have done it before but frankly it has been so long that i have forgotten.

Maybe Stephen can tell us how he does his, as far as the repeating and turning to the next position because i need a refresher myself!

[steve]

I'll give it a shot Jack...
I am just going to run through the process as I do it, I may be repeating stuff people already know.
My indexer is X parallel.

Refering to the picture Thistle Post layout.JPG, Y axis 0" is at the bottom or the drawing page, this is where I zero my Y axis after turning the basic shape.
You will notice that the vector that is the toolpath goes below the page on one vector but not the other. As long as the bit moves far enough away as to not hit the work on the return trip it doesn't mater if it goes to 0" or farther right.

The two circles with the cross hair represents the bit size, outer circle for the overall dia. and the inner circle is the depth of cut. I use this to determin where to have the bit enter or leave the turning.

As for positioning the bit where you want it, I do it from the keyboard. Once I have a routine I will write lines in the cutting file to position the bit and give new values to Y axis where necessary. Also the center of the cutting portion of the bit will have to be "zeroed" at the center of the turning, verticly that is.

REMEMBER the machine has no idea you are working on the side of the turning instead of the top. If you stop the machine while the bit is cutting it will, of course, go to the safe Z location, thus wrecking the turning.

For doing reeds...
As for how many passes and how much to turn the B axis, you'll have to figure that out your self. You need to divide the circumference of the turning by the dia. of the bit your using. That gives you the number of passes ( round up or down). Next divide 360 deg by the number of passes, the resulting number is the deg. to turn B axis after each pass.
In the picture after each pass I moved B 16.36Deg.


You will need to write the code yourself and repeat the toolpath and B movment for each pass.


Cleas as mud?

[dana_swift]

The documentation on making custom post processors comes with Aspire. It is easy to do, although the first time there its a tad confusing. An experiment or two cleared up the confusion for me. The post processor for Aspire is just a text file you can examine and edit easily in Notepad++, especially when you read the good documentation Vectric provided.

I have gotten so accustomed to setting things up "my way" that I dont have any stock processors in use any more. I output documentation info, setup my indexer so the rotation rate of the indexer increases as the radius drops, etc. (I have posted that elsewhere on the forum.)

As I am equally interested in having a side cutting post processor, I would be happy to collaborate and post the result to the forum for everyone to use and enjoy. There is nothing on my plate that needs this technique at the moment, but this project should take a whopping half hour or so to have ready.

As to bits- I needed some custom 4" bits made by Centurion, now they are on their standard available parts. I needed them for deep pockets, and they are going to be perfect for this application. According to the folks at Centurion, 4" is a standard carbide blank they cut the bit flutes into. Pick a standard diameter. (Note 3" of a 4" bit protrude from the collett.. and with the 0.25 bits low feed rates are required to keep the bits from flexing and chattering, however they work wonderfully.)

Also Gary Beckwith sells some custom tapered bits that might be just what the application calls for, so there is a variable radius for a "rough cut" and a "fine cut". That probably warrants investigation, Gary are you reading this?

Jack.. yes you can "create a profile toolpath" and it will solve the problem once. A custom post will make anything with the development effort confined to the generation of the post file. If I somebody only wants to do this technique once I would recommend your method.

D

[dana_swift]

I have been thinking about it some more, probably the side cut strategy can be enhanced with a "roughing" side cut strategy, and a "final cut" strategy where Aspire would follow the side cut method with a traditional Z strategy using a V bit so the deep V cuts in a toolpath could be cut correctly also.

The most difficult part of the side cut method it two zero routines are needed, one to locate the tip of the bit on the centerline of the indexer, and one to set the side of the bit against the centerline of the indexer from the Y direction.

Musing in public

D

[myxpykalix]

Stephen and Dana

Those instructions were great and very concise. BUT...(you knew that was coming..) here is one of the parts I keep forgetting as illustrated by your butchered drawing...

Regarding positioning...how do you know what length to make the "leg" of your toolpath from centerline to where it comes into contact with your material taking into account both the diameter of the bit and depth of cut, as represented by the section with the red question mark and the blue arrow?

I understand that you can start from anywhere, what i was trying to figure was how do you determine that length of "leg" so as not to go too deep into your material?

Also, as illustrated by the yellow arrow how do you determine where to place your bit so as to follow the contour of the part? I am assuming you use the the whole model (in essence) to help determine this?

Am I overthinking all of this? I have a tendency to do that, when i forget things. Once i recall (or am reminded or taught) then i understand.

Thanks for helping guys!:)

[myxpykalix]

As i was composing my clumsy questions and drawings you were saying kind of the same things (in a more concise way)....

whats that old saying..."great minds think alike"?

[steve]

Jack, that is what the two circles with the cross hairs are for, that is the bit. The inside circle is the bearing size (the bearing should be taken off in use). The outside circle is the overall size of the bit. I use this bit drawing to locate the position of the "legs" to and from the work.
I use part of the original vector to make a closed vector and set the bit to cut inside the vector.

[kubotaman]

Stephen, I am catching on to what you talking about when looking at your drawing. Will you please highlite in the drawing where you are zeroing the Y axis? That will help clear a few things I want to know. So am I to assume that when you make your vectors from your turning drawing it really is pocket cut done at Z being zero, set on the center of the stock, and y doing the cutting at the side at one level? Hope I am clear enough to understand!

[steve]

Dayrl, here is the revised picture. This is the actual drawing page. This would be a view from above the indexer with the headstock to the left and looking down.

Y axis 0" is the bottom of the page. Center of turning is 2.8284 inches from 0.
The toolpath in an inside profile cut, not a pocket cut.
It is a little hard to bend ones head around this stuff, basicly you have to think of everything sideways.
As for the Z axis it may be below 0", depends on the bit you are using. The center of the cutting portition of the bit will be at Z 0", not the bottom of the bit.

[kubotaman]

Stephen, I am about 97.89% understanding it now!!!! Sometimes I am not too smart since where I am there is absolutely no one to ask. I guess I should not have said a pocket cut. What I meant is a "Pocket cut" which has no depth of cut. You are correct to say a vector cut done on the inside with a offset of the radius of the cutter minus the depth of cut. Correct? So in your drawing the X axis is still in the original position, to the far right correct? The computer would know where the cutting vector starts and stops since it is working off the original file. If you would manually change bits you would then edit the cutting file to drop the Z axis down to center and Y would then be offset 2.8284 inches from center. Instead of physically off setting the Y axis couldn't you just edit the file? That way if any other cuts had to be made you don't have to reset the setup again? Hope I am clear. Thanks!!!

[myxpykalix]

WHUUT? Daryl, I was fairly clear till you posted the last thing, now i'm confused again! lol

Looking at your picture again Stephen i'm still confused by how to determine the depth of cut....

I think i'm starting to get it...am i on the right track? questions in pic

thanks stephen for your patience...

[kubotaman]

Okay since I have been thinking about this all day the light finally came on!!!!!!!!!!!!!!!!!!!!! Jack what I think you have to do is-"Example only"- Say the bearing is .5 inch in diameter and the cutter is .75 inch diameter. That would make the cutting edge .125 inch protrusion. Stephen's drawing shows the bearing and cutter diameter drawn on the center of the vecter that would be .375 inch from the spindle. The cut at this point would only skim the spindle since it is the same distance from the spindle as the radius of the cutter. Therefore it seems you would offset the cutter .15 to the outside of the vector which is towards the spindle. Hope I am correct??!! My problem I was trying to use the indexer all this time and really you stated in one of your responses to look at the spindle as a flat surface. Therefore all the indexer is doing is turning the spindle to the next necessary degree. BoyI sure hope I have it right this time.