[Goemon]

How do you guys program the lead-in when using Fusion 360 for Cam so that the tool doesn't get dragged through the side of the part at the start of a job?

I've been having problems with this lately. The simulation in CAM looks good and reports no collisions. I zero my machine and touch-off in linuxCNC but, when I click "run program" it drives the tool into the stock.

It completely ignores my lead-in setting and all the off-sets etc.

It happens in all toolpaths I've tried, but how do you guys avoid this in 2D pocket clearing, for example?

Every video tutorial I've watched skips over this bit like it doesn't matter but I'm clearly not understanding something key...

[joeavaerage]

Hi,
Lead-In and Lead-Out are the default toolpath strategies for Fusion. On the Linking Tab of the toolpath dialogue you can un-tick both Lead-In and Lead-Out.
I commonly use Ramp, and there are parameters that determine how aggressive that will be.

When I make circuit boards I will often use a 2D Contour path to cut a small hole, say 3.2mm with a 1.5mm endmill, it saves me having to change tools all the time.
Lead-In and Lead-Out will often even prevent the toolplath generation whereas Ramp circularly interpolates down nicely.

Craig

[joeavaerage]

Hi,

It completely ignores my lead-in setting and all the off-sets etc.

That rather sounds like the Heights are not set well. Do you use the Heights Tab of the toolpath dialogue?. Its very important that you know whether you have set the geometry to the
top outline of the part or the bottom, otherwise the toolpath will dive to the bottom at the first pass.

Craig

[dazp1976]

Hi,
That rather sounds like the Heights are not set well. Do you use the Heights Tab of the toolpath dialogue?. Its very important that you know whether you have set the geometry to the
top outline of the part or the bottom, otherwise the toolpath will dive to the bottom at the first pass.
Craig

I don't know what it's like in Fusion but in Inventor I have to watch those.
One of my dialogue boxes defaults as 'stock bottom' so if I set my stock top as 0 the box puts cut start at the bottom of the stock and the rest of the heights correspond.
If I run it it crashes tool trying to start job at bottom of stock.
For instance I set my tool on macine to the top of my cutting piece that's sayy 12mm thick and zero WCS. The posted G ccode would start cut at -12mm! and go down to -24mm!. Obviiously it should've been 0 to -12mm D'oh..
Yep!. It's a bit STUPID.
I have to remember to put the options in too. 'stock top' stock bottom 'model top' 'model bottom'.

Pockets I always lead helix.
Cutting from sides I always lead with added 'distance away from stock'.
Slots I ramp as gradual depth angles.
I try not to plunge at all if I an help it.

[joeavaerage]

Hi,

One of my dialogue boxes defaults as 'stock bottom' so if I set my stock top as 0 the box puts cut start at the bottom of the stock and the rest of the heights correspond.

I have not altered Fusion, to my knowledge it operates the way it does by default. The bottom of the toolpath is not defined, that is Fusion does not choose for you, you must
explicitly choose the StockTop OR StockBottom or what have you. Its still easy to confuse but I have not had a crash because of it, as I say you have to explicitly choose the bottom
of the toolpath.

Ramp, when used in small contour cuts is Helical, I don not choose helical explicitly but rather Ramp reverts to Helical if the feature is small.

Craig

[dazp1976]

Hi,
StockTop OR StockBottom or what have you. Its still easy to confuse but I have not had a crash because of it
Craig

Fortunately I spotted it during simullation run in my early days of learning Inv.
I have occasionally forgot to set it but I've got into a habit of checking the Gcode info line where it tells you tool #, D, and max Z depth.
If Z depth is way too low I know I ff'ed up.
It is rare, but I don't always simulate so needed a habit.

Anyhoo. Back to the OP. It's a learning curve. Make sure you are using correct post option for starters.
I would spend a day (or more) with a simplish design and go through the cam process page by page. Make slight changes to one little thing at a time and with every post you do, see what changes it makes.
You'll eventually know what everything does in a short time.

As for the video you saw. Skipping cam pages whether needed or not is a bad habit imv.

[Goemon]

The simulations don't help here because everything looks perfect there and it shows no crashes. But, it shows no lead-in.

Also, after the initial dragging the tool through the side of the stock (and breaking any small tools), it raises to the correct height and runs the rest of the job perfectly (on the machine, not the simulation).

This is why my assumption is that I did something wrong with the lead-in.

Based on what Joeaverage said, it sounds like I need to untick lead-in and try ramp as it does indeed look like it's ignored my settings and like it's trying to start from the part center (like there's no lead-in code at all).

I set the bottom height to the lowest area on the part face to be machined and the top is set to the top of the stock. I then have the retract height set 5mm above the stock top. Does this sound correct?

[dazp1976]

The simulations don't help here because everything looks perfect there and it shows no crashes. But, it shows no lead-in.
Also, after the initial dragging the tool through the side of the stock (and breaking any small tools), it raises to the correct height and runs the rest of the job perfectly (on the machine, not the simulation).
This is why my assumption is that I did something wrong with the lead-in.
Based on what Joeaverage said, it sounds like I need to untick lead-in and try ramp as it does indeed look like it's ignored my settings and like it's trying to start from the part center (like there's no lead-in code at all).
I set the bottom height to the lowest area on the part face to be machined and the top is set to the top of the stock. I then have the retract height set 5mm above the stock top. Does this sound correct?

Lead ins aren't that noticable in simulatuon if at default distances.

1. Could it possibly be going to an accidental 'safe Z' height first that's been set as a negative value?.
Mine stops at my safe Z > rapids to position > brings Z to job > leads in.
Has similar characteristic.

2. Do you have your 'home' set uup properly?
If it's not, (depending how yours posts code) the G28 at start of code goes home first tthen to job.

If you have a G28 G91 Z0 at the start it will go home first and then to start position.
Try changing this tto something like GO Z15 or something instead. This will now bring Z to 15 > Go to position > and then Z down to job start.

If that fails then it's back to scratching heads again.

[Goemon]

Lead ins aren't that noticable in simulatuon if at default distances.

1. Could it possibly be going to an accidental 'safe Z' height first that's been set as a negative value?.
Mine stops at my safe Z > rapids to position > brings Z to job > leads in.
Has similar characteristic.

2. Do you have your 'home' set uup properly?
If it's not, (depending how yours posts code) the G28 at start of code goes home first tthen to job.

If you have a G28 G91 Z0 at the start it will go home first and then to start position.
Try changing this tto something like GO Z15 or something instead. This will now bring Z to 15 > Go to position > and then Z down to job start.

If that fails then it's back to scratching heads again.

I was just looking at that. There's a bunch of settings in the post processor menu that I usually ignore. The drop-down menu for safe retract height defaults to G53.

If this overrides everything I do in CAM and the touch-off process in Linuxcnc then that would explain it (I think).

The other options are G28 and clearance height.

I don't have homing switches. I've been setting the home position manually for each axis.

I also just noticed that there's a warning for the NC program that says "work offset has not been specified. Using G54 as WCS.

I extra confused by this because I specified the WCS and all the heights options. I thought Microsoft was the world leader in unhelpful error messages but Autodesk makes them look like amateurs..

[joeavaerage]

Hi,
there are only two things that I bother with in the Post set-up. That is Safe Retracts is set to Clearance Height and Radius Arcs is set to On.
That works perfectly with Mach4.

Craig

[Goemon]

Hi,
there are only two things that I bother with in the Post set-up. That is Safe Retracts is set to Clearance Height and Radius Arcs is set to On.
That works perfectly with Mach4.

Craig

Once I did the two things you suggested it all worked like a charm. Thank you! I really appreciate it.

I really don't remember needing to set it to "clearance height" in the post menu last time I made new programs. Is this new?

It's usually left out on all the tutorials too, which is odd given it's importance.

[joeavaerage]

Hi,
no its not new....and its really related to the machine rather than Fusion.

Remember the setting is called 'Safe Retracts', and your choice is closely related to your machine. For instance you might decide that you want the Z axis to withdraw all the
way to the top of the travel irrespective of the workpiece heights. Thus the retract is based on the machine not the job.

Your choice and mine is to have the Z axis retract relative to the part being made, which in turn defines the Top of Stock and other reference planes. If you load the stock 5mm
lower in the vise then then entire job, including the Retract Height is lowered the same 5mm as well once you touch-off your stock.

To my knowledge the setting is 'sticky', as is the use of Radius Arcs, as I no longer ever set them, in fact very seldom do I ever look at the Post Options dialogue, the settings I have made
previously apply as default to any new job I create.

Craig

[dazp1976]

Nice one for getting there and sussing it Craig.
I never would have considered it because My Inventor cam defaults retract as 10mm above stock.
I generally get 15mm clearance > 10mm retract > 5mm feed > 0mm stock heights.
If I have clamps in rapid areas that's the only time I increase clearnce and retract both to 30mm.

I've never had it cam/post in a negative value.... Actually..That;s incorrect........... Unless I've lowered the feed height when cutting a smaller pocket inside an already deep cut pocket. Such as bearing blocks.
Even then though. My machine safe Z height stops Z at 30mm > It moves xy to start position > then plunges negative inside the pocket to feed height missing the stock.

If safe Z was off, then it would plunge into stock first > then try to go xy into start position. That's a crash.

There are so many variables that can catch people out.

[Goemon]

Hi,
no its not new....and its really related to the machine rather than Fusion.

Remember the setting is called 'Safe Retracts', and your choice is closely related to your machine. For instance you might decide that you want the Z axis to withdraw all the
way to the top of the travel irrespective of the workpiece heights. Thus the retract is based on the machine not the job.

Your choice and mine is to have the Z axis retract relative to the part being made, which in turn defines the Top of Stock and other reference planes. If you load the stock 5mm
lower in the vise then then entire job, including the Retract Height is lowered the same 5mm as well once you touch-off your stock.

To my knowledge the setting is 'sticky', as is the use of Radius Arcs, as I no longer ever set them, in fact very seldom do I ever look at the Post Options dialogue, the settings I have made
previously apply as default to any new job I create.

Craig

I saw that it keeps my last setting (in Fusion). That's nice so I won't forget a break more tools.