Extra long tools cause crash

[BBOwen]

I know this is a simple problem but I can't see the forrest for the trees. I work on a HAAS GR-510 router. This happens when running a multiple tool operation. The machine will go and change the tool to the long tool but, even though I put the maximum z height, the tool will not z up but come straight across running into the stock causing a crash. This happens when I run a regular length tool first and then switch to an extra length tool. If I run the extra lenth tool first it doesn't happen. What is going on?

[Ocean Lacky™]

Tool length offset for the second tool same as the first?

[Müřlıń®]

Use absolute retract and clearance?

[Hardmill]

Dbl check where zero is set and all your retract hgts. (abs/inc ?? )

What type of toolpath ??

 

 

PEACE

[BBOwen]

TLOs are all set right per tool. I don't ever change the default incremental setting on any of my settings. I always put the maximum retract height for tool changes. This always happens on a 3D surface tool path.

[Ocean Lacky™]

If you can, put it up on the FTP. I'm sure someone can help figure it out.

[John13]

quote:

---

I don't ever change the default incremental setting on any of my settings.

---

Shouldn't this be absolute, not incremental?

[Hardmill]

quote:

---

Shouldn't this be absolute, not incremental?

---

I agree with the smurf, its much safer that way.

 

Could someone :SMACK: me now

 

 

PEACE

[John13]

:climbing up a ladder:

 

:SMACK::SMACK:size; font color>

[Troy Gossett Indepak Inc.]

It happens on the second tool because the Tool change is a canned cycle= z tchg height, xy tchg position, t chg, now the machine is at Z tchg Height and your code is most likely G0 G17 G90 G54 X*.*** Y*.***; If your tool length requires the Z to be above the Tool change position it will crash the part unless you tell the Machine to go to Z clearance first.

 

I'm pretty sure if you set Clearance to Absolute like stated above should solve your problem.

[Bryan Johnson]

Because on most machines, the toolchange position is above the workpiece, most posts are setup to always move XY first and then Z after the toolchange.

 

if (at the machine), your toolchange position is below the top of your part, changing the Clearance setting will not help.

 

You will need to modify the post to output the Z first and then the XY after each toolchange, or using a reference point might work.

[Piglet Trespassers William]

Use home position feature

~~~~~~~~~~~~

Home position dialog box

 

 

The home position is a location on the machine tool where the tool returns for tool changes and at the end of the NC program. The source of the default home position is specified in the control definition. It can come from the machine definition, the toolpath defaults file, or, for Mastercam Lathe, from the tool definition. Use this dialog box to override the default for an operation. Specify the new home position in either of three ways:

 

Enter coordinate positions directly in the fields. Enter coordinate values relative to the current Tplane and Tplane origin.

 

Choose From machine to read the home position from the machine definition.

 

Choose Select to return to the graphics window and select a point. Mastercam will automatically enter its coordinates in this dialog box.

 

In addition to a home position, Mastercam also lets you set reference points, which are intermediate points the tool will move to between the home position and the start or end of a toolpath.

 

Learn more about...

Home positions and reference points

 

Reference points dialog box

 

Toolpath parameters tab (Mill/Router)

 

Toolpath parameters tab (Lathe)

[Piglet Trespassers William]

Reference points dialog box

 

 

 

A reference point is a location that the tool moves to between the home position and the start or end of the toolpath. You can create separate reference points for both approach and retract moves. Use this dialog box to set reference points for the current operation, or to set default reference points for an axis combination within a machine definition.

 

First, select the type of reference point to set. Select the Approach or Retract check boxes to enable the reference point feature for that move. If you are setting lathe defaults, you can also define separate sets of reference points for ID and OD work. (When you turn on reference points for a Lathe toolpath, Mastercam automatically selects the right set of points.)

 

Second, set the coordinates of each point. Use any of the following techniques.

 

Type the coordinate positions directly in the dialog box fields. Use the X-Y-Z check boxes to activate each axis. For example, if X and Y are cleared and only Z is selected, the tool will rapid straight up to the specified Z-height at the end of the toolpath with no change in X or Y.

 

If you are setting reference points for an operation, choose the Select button to return to the graphic window and select a point.

 

If you are setting reference points for an operation, you can also choose From Machine to read the default value from the machine definition.

 

Choose Absolute to set the reference point relative to the origin (0,0,0) or choose Incremental to set the reference point relative to the first/last move in the toolpath.

 

To quickly set the same point for both approach and retract moves, use the arrows to copy the values from one side to the other.

[Müřlıń®]

On HAAS control be sure to use G28 and send the z to the top.

[Santa Fe]

I had the same problem and what I did was to modify the post so at every tool change it will include a Z home comand before the tool change and again after the tool change.

ex.

G91 G28 Z0.

M6 T2

G91 G28 Z0.

G0 G90 G54 X??? Y??? S???? M3 (at this move tool is allways at maximum height)

G43 H2 Z1.0

.

.