Welcome to ModelEngineMaker !If you have problems registering or logging in, please use the contact menu option to request assistance.
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.
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!Quote from: zeeprogrammer on May 24, 2020, 04:56:48 PMWith 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.
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.
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?
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
Zee:I was mostly going off your previous CamBam plot:Quote from: Hugh Currin on May 24, 2020, 10:17:11 PMSorry 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.
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.
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.
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.
CamBam doesn't support facing. I would need to insert the needed g-codes into the file.
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.
Quote from: zeeprogrammer on May 25, 2020, 01:49:52 PMIt'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.