From Manual to CNC - Sherlines

[kvom]

You can declare the tool radius a tenth smaller than the radius to cut to avoid math errors in CAM.

[Jasonb]

But is that likely to stop the chatter when a tool goes into a radius the same as the cutter? and what doe sit do to the O/A size of the part

Since I have got the CNC I have taken to drawing up any parts I want to make on it with a larger fillet radius than the tool I think I'm likely to use.  eg where I may have specified a 3mm radius as its a reasonable round number I now find I go for 3.25 or 3.5 if I'm thinking of using a 6mm cutter, No doubt you would be thinking of drawing 1/16, 1//8" radius but probably need to think about drawing 0.035 or 0.070" radius as it is mostly easier to alter the part and use a standard cutter

[john mills]

what ever is on the program the tool will not like cutting the full radius the same or very near the radius of the cutting tool by making the radius bigger than the tool like you suggest is good .you could always come back with a smaller tool and just finish that bit with a separate cut.
when programming old machine which old controls using cutter compensation a tangental radius had to be added
to internal corners for it to work the machine did not read ahead i would put a 5.5 rad for a 10mm end mill but any end mill 10mm dia that had been ground could be used as long as the radius was put in the offset.the bigger the difference from the radius the better they will cut.

[zeeprogrammer]

Very interesting discussion. Thanks for that.

I understand the issue regarding cutting the radius with a tool of the same radius.
Easy enough to make a change to the drawing.

I tried a couple of things today.
The first was to turn on the tool tip radius offset. That was a complete failure. Most of the tip of the part did not get cut and for some reason, neither was the side cut.
That's on the left side of attached picture. So forget that.

Then I turned tool tip radius offset off again but set the home position such that the tool tip Z was centered on the end of the part and the X was past the centerline by the radius of the tool tip.
Better but still off.
That's on the right side of the attached picture.
Not that shape of the part end that I wanted.

In any case, this seems to be about understanding where the virtual tool tip is, where the actual cutting edge is, and where home is defined.
When it comes to the virtual and actual tool tip...most of what I've come across has been about a left or right hand cutting tool.
In this case I'm using a tool that looks like a parting tool with its tip rounded over. No 'left' or 'right'. (Which I think is why I want the tool tip radius offset off.)

2nd attachment shows the tool paths.
Passes up to the lower green line are roughing passes.
The last green line is the finishing pass.
So where should home be? To the right of Y and along X? On Y and X? Past X for either Z?
But I don't know (yet) what the post processor does.

BTW CamBam generated two finishing passes (I believe someone mentioned it should be one.)
Could this be a mismatch between the roughing clearance profile and the depth of cut for the finish?

I really appreciate all the comments. Helps a lot.

I think I'm making progress. That's what counts.

[john mills]

Hi Zee
when you set your xo front of the tool is on the centre line end of the tool will produce correct x dia you want
z 0 is still the end part is z-.these should remain the same what ever you are machining only adjust x togged correct x dia error.
then it is work on your part program to get the right part that you want.
the tool radius is on the approach side you are cutting from tail stock end to chuck just think of the radius on that side .
now with out cutter compensation you should get a tool path  that will leave a little bit at the centre radius of the tool .then the overall dia should be correct (   x0 was set )the only error will be the radius on the part will have error ,The tool will cut at different points around the radius of the tip but  the general shape should be there .
when you turn on cutter comp it should correct those errors by giving only slightly different path
so try plotting with out comp on  see if you have the right shape  don't change x0 or z0 that changes the position of the whole shape .whe that is right .try with comp on and see what the changes are to the tool path.
if that is not right you have to go back to see how the program starts and gets the compensation work .see if you can get the plot to look right.

John   

[zeeprogrammer]

Thanks John. You gave me an idea.

I wrote a (very dirty) little program to plot the toolpaths and output the points so they were easier to analyze.
1st pic is a screen shot of the program.
The yellow crosshairs are the beginning of a cut. The length of a hair is the diameter of the tool tip.
Think of the crosshair as a circle representing the cutter.
The green lines are the axes.
Ignore the two crosshairs at the very top. They're a remnant of testing the drawing of the crosshair.
You can see that the cutter crosses the X axis.

With tool radius off I saw that the tool tip never crossed the X axis.
With tool radius on (as shown in the attachment), the tool tip cross the X axis at the end of the part.
I homed the cutter in X by moving the tool tip against the flat of the part.
The stock is 1/4" hex brass. So home was set to 0.125".
I homed the cutter in Z by moving the tool tip against the faced end of the part and setting it to 0.

2nd pic shows the result.
The left end was the very first attempt. The right end is the result of this attempt.
The diameter of the finial measured 0.246 (perhaps 0.245) which was pretty spot on according to my drawing.
You'll note the left end is significantly smaller. I don't know why. I don't care.

However, there's still a slight flat on the very end of the part (right side).
I think it's because of the cutter itself (and possibly an inaccurate Z home). The cutter was homemade and I don't think its tip is perfectly round.

But overall I think it worked. I certainly got a better understanding.

One thing that worries me is having the raw stock pushed into the chuck as cuts are made.
I don't think that happened this round (very light cuts) but I think contributed to the failure on my first attempt (left side).

3rd attachment is the g-code file.
4th attachment is the output of my little program...
1st column is whether the move is G0, G1, or G2.
2nd and 3rd column are the X and Z coordinates. You can see that X goes negative.
4th and 5th columns are the coordinates used to create the graph. This is after scaling but before applying offsets to keep the drawing from the edges.

Thanks everyone for your help. I learned a lot.

[Hugh Currin]

Zee:

Now I'm quit confused. I can't find anywhere in CAMBAM to set "tool radius" on or off? I found "Lathe Tool Radius Offset" in the CAMBAM documentation related to post processors but can't see how to apply it. It doesn't seem to show up in any of the lathe posts. Where are you setting this?

I think CAMBAM outputs a tool path for the center of the tool, center of tip diameter. This is the same as it outputs the path for the center of the tool for milling. As long as the tool diameter is given to the controller this should work without any tool compensation.

Looking at the tool path plot on your previous post. I think this worked OK. If you take this path as the center of the tip diameter it starts cutting at the center of rotation. The top of the profile should be cut. It then follows the profile to the left as it should. It does look like it's not reaching the bottom of the cut on left side. It's like the tool is too large to get to the bottom. But this could be the way I'm seeing the drawing. If I'm seeing it correctly reduce the tool radius and see if it goes deeper. But the start of the cut at the far right should be OK.

You might try a lead in motion. This feeds the tool into the starting cut. Also, if you think the part may be slipping in the chuck you may not want to cut from the center. There's no relative motion at the center of rotation so cutting is like using a drill, takes some force. Starting the cut at the center of rotation could give a "large" cut to start. You could try taking a facing cut first to final size. Start from the OD and feed in to the center, like you would with a manual machine. Then run the profile cuts.

Starting past the center of rotation may be counter productive. This will put excess force on the part towards the chuck. If it tends to slip in the jaws this will make that worse. (yes, I did suggest this but after further thoughts I think it may be a bad idea.)

Good progress, congratulations.

With tool radius off I saw that the tool tip never crossed the X axis.
With tool radius on (as shown in the attachment), the tool tip cross the X axis at the end of the part.
I homed the cutter in X by moving the tool tip against the flat of the part.
The stock is 1/4" hex brass. So home was set to 0.125".
I homed the cutter in Z by moving the tool tip against the faced end of the part and setting it to 0.

[zeeprogrammer]

Thanks Hugh.

Now I'm quit confused. I can't find anywhere in CAMBAM to set "tool radius" on or off? I found "Lathe Tool Radius Offset" in the CAMBAM documentation related to post processors but can't see how to apply it. It doesn't seem to show up in any of the lathe posts. Where are you setting this?
Sorry about that. I meant Lathe Tool Radius Offset. It's in the System tab. Select the post processor (Mach3-Turn in this case) then scroll down in the lower pane. Same place where you set whether X mode is radius or not.

I think CAMBAM outputs a tool path for the center of the tool, center of tip diameter. This is the same as it outputs the path for the center of the tool for milling. As long as the tool diameter is given to the controller this should work without any tool compensation.
That was in part why I wrote my dirty little program. Seeing the tool paths in CamBam didn't tell me what effect the post processor had (if any). And, I couldn't tell by the plot if I was seeing the 'center' of the tool tip or the cutting edge. Keep in mind, that attachment showing the plot is my program, not CamBam.

Looking at the tool path plot on your previous post. I think this worked OK. If you take this path as the center of the tip diameter it starts cutting at the center of rotation. The top of the profile should be cut. It then follows the profile to the left as it should. It does look like it's not reaching the bottom of the cut on left side. It's like the tool is too large to get to the bottom. But this could be the way I'm seeing the drawing. If I'm seeing it correctly reduce the tool radius and see if it goes deeper. But the start of the cut at the far right should be OK.
I'm not sure I follow. It did not start cutting at the center of rotation. It started from just outside the surface of the stock, bringing the part to diameter. Then worked along the tip, then made the final roughing and finishing cut starting at axis of rotation. I think the reason you mentioned 'not reaching the bottom of the cut on the left side'...CamBam just shows the tool path and not the shape of the tool. In my program, the crosshair represents the shape of the tool. Just pretend it's a circle. (I had enlarged the part radius a bit so the cutter wasn't cutting along too much of its circumference.

You might try a lead in motion. This feeds the tool into the starting cut. I've seen references to 'lead in'. I don't know anything about yet or what it means.Also, if you think the part may be slipping in the chuck you may not want to cut from the center. There's no relative motion at the center of rotation so cutting is like using a drill, takes some force. Starting the cut at the center of rotation could give a "large" cut to start. You could try taking a facing cut first to final size. Start from the OD and feed in to the center, like you would with a manual machine. Then run the profile cuts.
If I understand you right, I think that's what was happening. That is, starting from OD, cutting right to left, and slowly moving towards axis of rotation. Or if you look at the plot from my program...start at the lower right. It moves left then starts over a litte closer to X.

Starting past the center of rotation may be counter productive. This will put excess force on the part towards the chuck. If it tends to slip in the jaws this will make that worse. (yes, I did suggest this but after further thoughts I think it may be a bad idea.)
It only goes past center of rotation during the last roughing cut and the finishing cut. By which time there is little part left. I think it was possible the part got pushed into the chuck on early attempts because the depth of cut was too large.

Good progress, congratulations.
Thanks!

With tool radius off I saw that the tool tip never crossed the X axis.
With tool radius on (as shown in the attachment), the tool tip cross the X axis at the end of the part.
I homed the cutter in X by moving the tool tip against the flat of the part.
The stock is 1/4" hex brass. So home was set to 0.125".
I homed the cutter in Z by moving the tool tip against the faced end of the part and setting it to 0.
After finding home I moved the cutter away from the part before starting the g-code program.

[john mills]

it looks like you can see whats happening now .
the idea of a facing cut is what you would normally start a programme but as the roughing cuts have removed most of the metal as  the program progresses that is not needed for the finish cut the tool going past the centre is because it is cutting at the side of the tool at this time not at the end.
moving in the chuck is problem from the force of the cut.on bigger industrial machines with big powfull hydraulic chucks it happens .machining harder tools steels even more likely turning whith a centre means as it moves the centre comes forward until thing get in the way the tool can come into the live centre or when there is not much room parts of the machine can bump.often using soft jaws  they can be machined with a step ,the material has tone against something so it can not move .
good to see you can see whats happening now.   

[john mills]

Hugh
the calculations are done as from the centre of the tool radius but the tool is set to the edge either the side z0 or the front of the tool x    when milling the x0  y0   are set in the centre of the tool.
hope that helps.   
         John

[Hugh Currin]

Zee:

I was mostly going off your previous CamBam plot:

Sorry about that. I meant Lathe Tool Radius Offset. It's in the System tab. Select the post processor (Mach3-Turn in this case) then scroll down in the lower pane. Same place where you set whether X mode is radius or not. No problem. I found it via your direction. I made up a small test part and had CamBam generate lathe code for it. I ran two versions, one with Lathe Tool Radius Offset true and one false. I couldn't see a difference in the tool paths. So, I compared the two *.nc files and found the only difference was the time stamp. Thus, this parameter doesn't seem to do anything, but I don't know what it is supposed to do? The description in CamBam documentation isn't clear to me. Can you explain what it's supposed to do?

I'm not sure I follow. It did not start cutting at the center of rotation. It started from just outside the surface of the stock, bringing the part to diameter. Then worked along the tip, then made the final roughing and finishing cut starting at axis of rotation. I think the reason you mentioned 'not reaching the bottom of the cut on the left side'...CamBam just shows the tool path and not the shape of the tool. In my program, the crosshair represents the shape of the tool. Just pretend it's a circle. (I had enlarged the part radius a bit so the cutter wasn't cutting along too much of its circumference. My bad, I'm not explaining things well. I was thinking of the final roughing and finishing cuts. They do cut at the center of rotation, but after the previous cuts it's taking little material. Although that depends on how much stock is left to cut on the right end. Looking at the CamBam plot above, the center of the tool radius, plotted points, do start at the center of rotation for the last rough and the finishing cuts. It should be cutting the whole profile.

In this plot again, it looks to me like the tool path doesn't reach the center of the circular profile on the left end. This is what I meant in my previous email. It's hard to see this in your plot as the profile itself isn't shown. If you increased this profile arc you've likely fixed this.

I've seen references to 'lead in'. I don't know anything about yet or what it means. This screen shot (attached) of CamBam for my trial part shows straight lead in and lead out moves. Here just moves so I know how it's approaching a cut. Lead in and out are more useful in milling where you can arc into and out of a cut leaving no noticeable tool mark where the cut starts and ends.

If I understand you right, I think that's what was happening. That is, starting from OD, cutting right to left, and slowly moving towards axis of rotation. Or if you look at the plot from my program...start at the lower right. It moves left then starts over a litte closer to X. What I was thinking of was a facing cut to size on the end of the part. Before taking the diameter down make a cut from outside to the center on the end of the part. But as you say, it probably wouldn't help considering the roughing cuts to reduce diameter.

It only goes past center of rotation during the last roughing cut and the finishing cut. By which time there is little part left. I think it was possible the part got pushed into the chuck on early attempts because the depth of cut was too large. But any motion past the center line will just have the tool rubbing. But you are right, it probably doesn't matter. How did you force the cutting beyond the center line anyway?

Thanks.

[Hugh Currin]

John:

Yes, I agree. Thanks.

Hugh
the calculations are done as from the centre of the tool radius but the tool is set to the edge either the side z0 or the front of the tool x    when milling the x0  y0   are set in the centre of the tool.
hope that helps.   
         John

[zeeprogrammer]

Zee:

I was mostly going off your previous CamBam plot:

Sorry about that. I meant Lathe Tool Radius Offset. It's in the System tab. Select the post processor (Mach3-Turn in this case) then scroll down in the lower pane. Same place where you set whether X mode is radius or not. No problem. I found it via your direction. I made up a small test part and had CamBam generate lathe code for it. I ran two versions, one with Lathe Tool Radius Offset true and one false. I couldn't see a difference in the tool paths. So, I compared the two *.nc files and found the only difference was the time stamp. Thus, this parameter doesn't seem to do anything, but I don't know what it is supposed to do? The description in CamBam documentation isn't clear to me. Can you explain what it's supposed to do?
Odd. When I did it the files were quite different. Attached is a screenshot showing a portion of the difference between the two files. (My editor has a 'file difference' feature.) Here's an explanation from CamBam about the Lathe Tool Radius Offset... http://www.cambam.info/doc/plus/cam/Lathe.htm  (Scroll to near bottom). You won't see a change in the tool paths drawn in CamBam.

I'm not sure I follow. It did not start cutting at the center of rotation. It started from just outside the surface of the stock, bringing the part to diameter. Then worked along the tip, then made the final roughing and finishing cut starting at axis of rotation. I think the reason you mentioned 'not reaching the bottom of the cut on the left side'...CamBam just shows the tool path and not the shape of the tool. In my program, the crosshair represents the shape of the tool. Just pretend it's a circle. (I had enlarged the part radius a bit so the cutter wasn't cutting along too much of its circumference. My bad, I'm not explaining things well. I was thinking of the final roughing and finishing cuts. They do cut at the center of rotation, but after the previous cuts it's taking little material. Although that depends on how much stock is left to cut on the right end. Looking at the CamBam plot above, the center of the tool radius, plotted points, do start at the center of rotation for the last rough and the finishing cuts. It should be cutting the whole profile.

In this plot again, it looks to me like the tool path doesn't reach the center of the circular profile on the left end. This is what I meant in my previous email. It's hard to see this in your plot as the profile itself isn't shown. If you increased this profile arc you've likely fixed this. The profile is the red line. I don't understand why you say the profile itself isn't shown. I did enlarge that arc a bit (not shown) but didn't see any real difference.

I've seen references to 'lead in'. I don't know anything about yet or what it means. This screen shot (attached) of CamBam for my trial part shows straight lead in and lead out moves. Here just moves so I know how it's approaching a cut. Lead in and out are more useful in milling where you can arc into and out of a cut leaving no noticeable tool mark where the cut starts and ends.
Ah. Thanks.
If I understand you right, I think that's what was happening. That is, starting from OD, cutting right to left, and slowly moving towards axis of rotation. Or if you look at the plot from my program...start at the lower right. It moves left then starts over a litte closer to X. What I was thinking of was a facing cut to size on the end of the part. Before taking the diameter down make a cut from outside to the center on the end of the part. But as you say, it probably wouldn't help considering the roughing cuts to reduce diameter. CamBam doesn't support facing. I would need to insert the needed g-codes into the file. In this case, I had faced the part on my other lathe. Not the best idea as accuracy can suffer but was good enough for this experiment.

It only goes past center of rotation during the last roughing cut and the finishing cut. By which time there is little part left. I think it was possible the part got pushed into the chuck on early attempts because the depth of cut was too large. But any motion past the center line will just have the tool rubbing. But you are right, it probably doesn't matter. How did you force the cutting beyond the center line anyway? I'm not sure about that. By the time the final roughing cut and the finishing cut start, the profile will have a series of steps in it from all the prior roughing passes. Then, as the tool tip moves along the profile, the steps are smoothed out. Think of the tool tip as a circle. It has to get past the center line in order for the left edge of the tool tip to cut. Note that the actual part of the tool tip that cuts moves as the tool tip 'rounds the corner' of the profile. The Lathe Tool Radius Offset made the difference. Setting it true caused the tool tip to go past the center line. What's curious to me...with the offset false there was still code showing the tool tip going past the center line but only by 1 or 3 thou. With the offset true, the tool tip went past the center line by the radius of the tool tip, which was what I wanted.

From what I can tell, CamBam plots the center of the tool. The post processor can make additional changes to the paths the tool takes depending on parameters (such as the lathe tool radius offset). This is why I wrote my little program to display the 'new' tool paths and give some sense of where the edge of the cutter is. In hindsight, I didn't really need my little program. Viewing the output file showed what was happening to the tool tip.

Thanks again, Hugh, John, and all the rest. All of this was very helpful (as well as fun and satisfying). 

[Hugh Currin]

Zee:

Comments below:

Odd. When I did it the files were quite different. Attached is a screenshot showing a portion of the difference between the two files. (My editor has a 'file difference' feature.) Here's an explanation from CamBam about the Lathe Tool Radius Offset... http://www.cambam.info/doc/plus/cam/Lathe.htm  (Scroll to near bottom). You won't see a change in the tool paths drawn in CamBam.

Yep. I wasn't saving the post processor correctly. Now it looks like a radius difference in X and Z which would match the desctiption CamBam gives. The description makes more sense now.

It's hard to see this in your plot as the profile itself isn't shown. The profile is the red line. I don't understand why you say the profile itself isn't shown.

Here I was referring to the plot from the program you wrote. I see the profile on the CamBam plots but not in the graph from your program.

CamBam doesn't support facing. I would need to insert the needed g-codes into the file.

I agree, I couldn't find an easy was to do a facing cut. Seems like there should be a way but I couldn't find it. Tried a milling profile cut which looked OK but the G-code didn't come out right. Could hand code it but that is a pain, particularly if you modify anything.

From what I can tell, CamBam plots the center of the tool. The post processor can make additional changes to the paths the tool takes depending on parameters (such as the lathe tool radius offset). This is why I wrote my little program to display the 'new' tool paths and give some sense of where the edge of the cutter is. In hindsight, I didn't really need my little program. Viewing the output file showed what was happening to the tool tip.

It seems like this is true. The machine controller makes additional adjustments. I'll likely use the nose radius, leave the "Lathe Tool Radius Offset" true, and enter the nose radius in LinuxCNC. That seems to work for my setup.

A good learning experience all the way around. Thanks.

[zeeprogrammer]

It's hard to see this in your plot as the profile itself isn't shown. The profile is the red line. I don't understand why you say the profile itself isn't shown.

Here I was referring to the plot from the program you wrote. I see the profile on the CamBam plots but not in the graph from your program.

Ah yes. I didn't bother to plot the profile. My little program was built from other programs I'd written in the past. All I had was the ability to plot straight lines, not circles or ellipses. Plus, I would have had to figure out how to input the profile (and scale it correctly) or figure out how to read and plot the DXF file.

In fact, I only plotted G1 movements. G0 seems to be used for rapids to clear the part. G2 requires a different Bresenham algorithm which I didn't want to bother with. G2 only came into play during the last roughing cut and during the finishing cut. (I suppose I could find some Visual Studio routines but I used what I'd written years ago.)

Lastly, I was more interested in seeing what was going on to the right of the part. The crosshair represented the tool tip so you can actually 'see' the profile by 'connecting' the appropriate hair ends (and squinting). If you draw a circle around and encompassing that tip in the neck...that would be the radius of the neck. The radius of the neck is slightly larger than the radius of the tool tip (crosshair) but the resolution of the system prevents seeing very small movements.

Thanks again. I'm very glad if you found all this useful.