Optirest toolpath showing collisions

[JB7280]

I have an opti toolpath, and it's showing a number of collisions.  I have looked and looked, and tried changing a number of different settings, and it doesn't appear that they're actually even collisions, but maybe I'm missing something.  Am I missing something?  Maybe a tolerance setting somewhere?  When it shows the collisions, the tool is not even engaged in the part.  What am I doing wrong?   The problem is in the first toolpath, operation #2

 

It's a big model, but I added some material to try to obscure it a little.

 

https://www.dropbox.com/s/ap92rcn9opn77ej/modfied solid.mcam?dl=0

[ajmer]

it must be a dog leg verify issue

 

change linking to this and it will not happen

 

or change control def to this

 

depending on what your machine actually does

 

 

 

 

[Colin Gilchrist]

Do you happen to have Wireframe visible on the Mastercam screen? The Wireframe Checkbox is disabled by default in the Verify and Simulation, but it may be doing a collision check in the background. Also, same story for surfaces, if they're left visible. 

I always create a separate solid which is used for "Verify Workpiece" only. That way I can put chamfers on the Verify solid, but use the "Toolpath Solid" with sharp edges, to drive the Contour Chamfer paths.

[JB7280]

31 minutes ago, ajmer said:

it must be a dog leg verify issue

change linking to this and it will not happen

I will give that a shot in the morning.  Thanks.

12 minutes ago, Colin Gilchrist said:

Do you happen to have Wireframe visible on the Mastercam screen? 

I don't think so but I'll check that in the morning Colin.  Thanks for the suggestions!

[crazy^millman]

Thing Ajmer didn't mention is make sure the linking feed rate is at least the same feed rate as your operation or back feed rate to reduce run time. I will run as much as 2500 inched per minute on large machines and on smaller machines 400 to 800 ipm. The higher the feed rate on the linking the more I will adjust the part clearance and arc fit.  

[JB7280]

14 hours ago, Colin Gilchrist said:

Do you happen to have Wireframe visible on the Mastercam screen? The Wireframe Checkbox is disabled by default in the Verify and Simulation, but it may be doing a collision check in the background. Also, same story for surfaces, if they're left visible. 

I always create a separate solid which is used for "Verify Workpiece" only. That way I can put chamfers on the Verify solid, but use the "Toolpath Solid" with sharp edges, to drive the Contour Chamfer paths.

I actually don't even have any wireframe on this part yet.  But thank you

[gcode]

Before you change the rapids definition on your machine definition find out if your machine doglegs or not

If you don't know it's very easy to test

MDI

G0 X10. Y5.

If your machine doglegs it will run to X5 Y5 then X10

If it doesn't dog leg it will hit X10 Y5 at the same time running in a straight line

It is very important that the control def setting matches your machine's behavior.

Backplot does not simulate dogleg motion, but verify and machine sim do.

If your machine doglegs and you have rapids set to

"All axis arrive at destination simultaneously",  verify will not warn you of potential crashes

Verify will run in straight lines, but in real life your machine is doglegging

It will run great in verify but smash tools and wreck parts in real life

The opposite is also true

If you have Mastercam set to dogleg, Verify will drive you nuts reporting crashes

that aren't really there out on the machine.

Test this and get it set right. It's important.

 

 

[JB7280]

26 minutes ago, gcode said:

Before you change the rapids definition on your machine definition find out if your machine doglegs or not

If you don't know it's very easy to test

MDI

G0 X10. Y5.

If your machine doglegs it will run to X5 Y5 then X10

If it doesn't dog leg it will hit X10 Y5 at the same time running in a straight line

It is very important that the control def setting matches your machine's behavior.

Backplot does not simulate dogleg motion, but verify and machine sim do.

If your machine doglegs and you have rapids set to

"All axis arrive at destination simultaneously",  verify will not warn you of potential crashes

Verify will run in straight lines, but in real life your machine is doglegging

It will run great in verify but smash tools and wreck parts in real life

The opposite is also true

If you have Mastercam set to dogleg, Verify will drive you nuts reporting crashes

that aren't really there out on the machine.

Test this and get it set right. It's important.

 

 

Cool, thanks.  Changing that in the CD did fix the problem, though I did want to make sure it was actually replicating what the machine does.  So next time it's in between cycles I will check that out.  Thanks.

[Colin Gilchrist]

To handle "changing it in the Control Definition", it is important to note the following:

• There is a Checkbox in "General Machine Parameters", which tells Mastercam to use "the same RAPID RATE", for all Linear Axes. (If all three axes move at the same linear rate, you can set the value here.
• More often than not; your machine will have different Rapid Rates for each Linear Axis. (It is quite common to have faster XY, and slower Z, due to the mass of the machine that is being moved around.)
• To set different rates "per axis", you must uncheck that "Apply to all axes" button (one for Linear Axes, one for Rotary Axes), in General Machine Parameters.
• Then, you must double-click (properties dialog) each Axis, and set the specific speed for that Linear or Rotary Axis.
• Mastercam will then use the Control Definition settings (each axis moves at maximum feedrate independently), to show you more accurate 'machine behavior' in Backplot/Verify/Simulation.

 

[JB7280]

21 minutes ago, Colin Gilchrist said:

To handle "changing it in the Control Definition", it is important to note the following:

• There is a Checkbox in "General Machine Parameters", which tells Mastercam to use "the same RAPID RATE", for all Linear Axes. (If all three axes move at the same linear rate, you can set the value here.
• More often than not; your machine will have different Rapid Rates for each Linear Axis. (It is quite common to have faster XY, and slower Z, due to the mass of the machine that is being moved around.)
• To set different rates "per axis", you must uncheck that "Apply to all axes" button (one for Linear Axes, one for Rotary Axes), in General Machine Parameters.
• Then, you must double-click (properties dialog) each Axis, and set the specific speed for that Linear or Rotary Axis.
• Mastercam will then use the Control Definition settings (each axis moves at maximum feedrate independently), to show you more accurate 'machine behavior' in Backplot/Verify/Simulation.

 

Thanks Colin, I was able to find the min/max feed and rapid rates for my machine, and I changed them in the MD.  On this machine, they do happen to be the same for all linear axes.    I thought I had the collision issue fixed, but unfortunately when I turned the precision slider back up to the middle, it shows collisions again.  Collision report shows that the collision is related to the shank.  Perhaps the geometry of the tool is incorrect.  It doesn't appear to be, but I'll try recreating it.

[Chally72]

4 minutes ago, JB7280 said:

Thanks Colin, I was able to find the min/max feed and rapid rates for my machine, and I changed them in the MD.  On this machine, they do happen to be the same for all linear axes.    I thought I had the collision issue fixed, but unfortunately when I turned the precision slider back up to the middle, it shows collisions again.  Collision report shows that the collision is related to the shank.  Perhaps the geometry of the tool is incorrect.  It doesn't appear to be, but I'll try recreating it.

 

Remember that even with a lot of work here,  you still can't match your real life scenario 1:1. Acceleration rates for each axis, even if your machine builder provided them, are in an unloaded state. Put 300lbs of fixturing on top of everything, and maybe suddenly the X is much slower to accelerate than the Y, and now you have dogleg motion that is entirely different than your dialed in Machine definition motion. This means something that just barely clears in Verify now clips your part in real life. For this reason, it's safest to convert rapids to feeds if you're going to be moving around between part features or stock without lifting the Z. 

[JB7280]

16 minutes ago, Chally72 said:

 

Remember that even with a lot of work here,  you still can't match your real life scenario 1:1. Acceleration rates for each axis, even if your machine builder provided them, are in an unloaded state. Put 300lbs of fixturing on top of everything, and maybe suddenly the X is much slower to accelerate than the Y, and now you have dogleg motion that is entirely different than your dialed in Machine definition motion. This means something that just barely clears in Verify now clips your part in real life. For this reason, it's safest to convert rapids to feeds if you're going to be moving around between part features or stock without lifting the Z. 

That makes sense.  Will definitely make sure there's enough clearance to accomodate.   Although where I'm seeing the collisions, it's just rounding the corner, in a feed move.  Not lifting or anything like that.

[JB7280]

The problem seemed to be something in the tool.  I was using a step file from Ingersoll to generate the shape of the tool,  I built the tool as a plain, 2" bull endmill and it ran the toolpath just fine.  Thanks for all the suggestions though, even though it was the tool, I learned a lot about the linking parameters, and settings in the opti toolpath!