Change start points

[Afshin karimi]

Hello there,

Is it possible to change start points of a 2d contour?

Like powermill stagger start points?

 

[cncasylum]

In your chaining manager for that tool path (geometry) right click on the chain you would like to edit, and you will find the start point option.

[Leon82]

You may have to uncheck start at middle of closed contours in lead in when you pick your new start point

[Afshin karimi]

27 minutes ago, Leon82 said:

 

I want to change all of the start point. I don't want my toolpath start at the same point every step. 

[JParis]

On round geometry, Helix Bore

otherwise, Contour >> Ramp

[Afshin karimi]

For holes Helix Bore is working. Tnx. 

But my problem is with Boss type feature, when you use contour with ramp option Arc filter is not working (in Helix Bore it's working well) and generate nc files with x,y,z and for some parts it reaches thousand of lines and take a lot of time for me to send it in my machine(Heidenhain 426). I'm looking for a solution to reduce the number of lines without loosing accuracy.

 

[Pgreenlaw]

2 hours ago, Afshin karimi said:

For holes Helix Bore is working. Tnx. 

But my problem is with Boss type feature, when you use contour with ramp option Arc filter is not working (in Helix Bore it's working well) and generate nc files with x,y,z and for some parts it reaches thousand of lines and take a lot of time for me to send it in my machine(Heidenhain 426). I'm looking for a solution to reduce the number of lines without loosing accuracy.

 

 

 

[crazy^millman]

23 hours ago, Afshin karimi said:

For holes Helix Bore is working. Tnx. 

But my problem is with Boss type feature, when you use contour with ramp option Arc filter is not working (in Helix Bore it's working well) and generate nc files with x,y,z and for some parts it reaches thousand of lines and take a lot of time for me to send it in my machine(Heidenhain 426). I'm looking for a solution to reduce the number of lines without loosing accuracy.

 

Use the arc3d chook on the toolpath and see if that fixes the bug in the filter setting. It has been tore up since about X5. Every version I do a 10” sphere test with the center of the sphere at zero.I will make a flow line it with a different ball endmills last test was a 2” ball endmill;. Filter it to the max. Normally I crash every version, but sometimes after 2 hours I will get the toolpath. Last test in 2022 was 310kb NCI or about 4000 lines of code. I then backplot that save geometry to a level. I then connect all the arcs aligning the start points to the same clocking. I make a 3D toolpath with that geometry and filter it with 50/50  .0001 tolerance G17, G18, G19 and make sure the filter settings in MCD on arc are set to make full arcs support arc on all planes. Now use the same filter settings on the flowline toolpath to cut the same exact shape. You will not get the same amount of code. 30 passes with 30 connecting moves should only produce 60 lines of code cutting an Sphere using a 2” ball endmill with the step over I use to test. Last pass should be exactly at -1.000 and with the filter settings and with a MCD configured correctly should be one line of code. Nope gets much worse the lower down the sphere you get. Math don’t lie unless you use Mastercam to filter the toolpath. I have seen this and been shut up so many times I quit bothering anymore. I get the more points is better all the time yet we have Thrasmillj g still using G2/G3 on non-taper threads. Before they broke the filters we would threadmill with a helix and get the same exact code without having to use this same Chook, but not anymore. Agin why is that? Because behind the scenes the math is tore up why we get scallops like we do. Why you have to filter to .-00001 of you really want mold quality finish. Problem is program because massive and you really bog down even the best computer. 
 

Go make Curves on the Sphere using Curve/Flowline and check them, The are all arcs so the CAD of the software is getting the math right, but so where in the Posting side of things does it get screwy real quick. Test a square and a Prymaid doing the same test they pretty much output the same code, but not a sphere. Again MATH don’t lie, but in Mastercam with filtering toolpaths it does. 

[Afshin karimi]

On 1/16/2022 at 8:38 AM, crazy^millman said:

Use the arc3d chook on the toolpath and see if that fixes the bug in the filter setting. It has been tore up since about X5. Every version I do a 10” sphere test with the center of the sphere at zero.I will make a flow line it with a different ball endmills last test was a 2” ball endmill;. Filter it to the max. Normally I crash every version, but sometimes after 2 hours I will get the toolpath. Last test in 2022 was 310kb NCI or about 4000 lines of code. I then backplot that save geometry to a level. I then connect all the arcs aligning the start points to the same clocking. I make a 3D toolpath with that geometry and filter it with 50/50  .0001 tolerance G17, G18, G19 and make sure the filter settings in MCD on arc are set to make full arcs support arc on all planes. Now use the same filter settings on the flowline toolpath to cut the same exact shape. You will not get the same amount of code. 30 passes with 30 connecting moves should only produce 60 lines of code cutting an Sphere using a 2” ball endmill with the step over I use to test. Last pass should be exactly at -1.000 and with the filter settings and with a MCD configured correctly should be one line of code. Nope gets much worse the lower down the sphere you get. Math don’t lie unless you use Mastercam to filter the toolpath. I have seen this and been shut up so many times I quit bothering anymore. I get the more points is better all the time yet we have Thrasmillj g still using G2/G3 on non-taper threads. Before they broke the filters we would threadmill with a helix and get the same exact code without having to use this same Chook, but not anymore. Agin why is that? Because behind the scenes the math is tore up why we get scallops like we do. Why you have to filter to .-00001 of you really want mold quality finish. Problem is program because massive and you really bog down even the best computer. 
 

Go make Curves on the Sphere using Curve/Flowline and check them, The are all arcs so the CAD of the software is getting the math right, but so where in the Posting side of things does it get screwy real quick. Test a square and a Prymaid doing the same test they pretty much output the same code, but not a sphere. Again MATH don’t lie, but in Mastercam with filtering toolpaths it does. 

It's working in many cases. I appreciate it. It help me a lot. 

[Colin Gilchrist]

Surface Finish Contour > "Start Length" Parameter, will "rotate" your entry/exit point, at the transition point of each individual Contour pass.

You should learn how to utilize the "Toolpath Filter". For Surface Finish Contour, you click on the "Total tolerance..." Button. Then, enable the Line/Arc Filter. Set your Total Tolerance to 0.001" (0.025 mm), and set the ratio to 50%/50%. (0.0125 mm for both).

Set your "Minimum Arc" in the filter to 0.01" (0.25 mm), and "Max Arc" to 8.0". (200-250mm)

I'd recommend using the "high-speed" transition, so you get a little "helical loop" from the last contour you cut (last depth), down to the "next depth". Remember that 'Start Length' will spread these points out as you step down the SFC Contour Passes.

[Colin Gilchrist]

To control "Depths" with SFC, you need to use the "Cut Depths" dialog box.

> Press the [Cut depths...] Button

Now, there is a bit of a secret here. For "Incremental", you have Adjustment to Top Cut, and Adjustment to other cuts.

> For "Adjustment to top cut", A Positive Number tells your cutter to "drop" that amount below the very top of the detected surface. Positive Number = Negative Depth (for this control only)

> For "Adjustments to other cuts", that values works the way "you think it should". A Negative Number = Negative Depth Adjustment. A Positive Number = Positive Depth adjustment. If you're depth cut value is "0.05 inches", and you can visually see you want to make "3 passes deeper", you'd subtract from the value. (if it was 0.0, change to -.150, to force 3 more depth cuts.)

This "Adjustment to Top Cut", is one of the weirdest, and trickiest options to understand in using any toolpath in this software. I think this is why so many people have switched over to "Absolute" values, when using Depth Cuts, for Surface Finish Contour. The problem is, if you end up changing your Plane or Geometry Depth, in any way, you've got to go and edit all the paths which use "Absolute" values. If you learn to properly use "Incremental Depths" (For both 2D Ops and 3D Ops in Mastercam), you have a lot more freedom to make a "global program change", where you can safely move an origin point, and all the Operations will regenerate without manual intervention.

[Afshin karimi]

• 17 hours ago, Colin Gilchrist said:

  Surface Finish Contour > "Start Length" Parameter, will "rotate" your entry/exit point, at the transition point of each individual Contour pass.

  You should learn how to utilize the "Toolpath Filter". For Surface Finish Contour, you click on the "Total tolerance..." Button. Then, enable the Line/Arc Filter. Set your Total Tolerance to 0.001" (0.025 mm), and set the ratio to 50%/50%. (0.0125 mm for both).

  Set your "Minimum Arc" in the filter to 0.01" (0.25 mm), and "Max Arc" to 8.0". (200-250mm)

  I'd recommend using the "high-speed" transition, so you get a little "helical loop" from the last contour you cut (last depth), down to the "next depth". Remember that 'Start Length' will spread these points out as you step down the SFC Contour Passes.

  Thank you. That's what I was looking for. appreciate it

[Colin Gilchrist]

37 minutes ago, Afshin karimi said:

• Thank you. That's what I was looking for. appreciate it

You're welcome, but keep in mind this is for Surface Finish Contour path only. You'll need to generate a "surface" for the boss. Not a big deal, but there is no option for this "start Length" when driving Wireframe Geometry with a 2D Contour path.