Recommended Posts

I’ve been working with a part for weeks now where the walls are drafted at .6 deg, and the walls are .1775 high.  The walls form teeth for a wave guide.  I’m using opti rough to take the cavity down to .020” remaining, then a swarf mill operation to finish the walls.  The problem is, the simulation shows the part to be perfect, but the physical part is over cut by .005.  I have a +\- .0005 tolerance and I can’t figure out how what’s wrong.  Anyone have any suggestions?

Share this post


Link to post
Share on other sites

+/-.0005" profile tolerance on a 5-Axis cut or wall thickness.

Share this post


Link to post
Share on other sites
38 minutes ago, [email protected] said:

I’ve been working with a part for weeks now where the walls are drafted at .6 deg, and the walls are .1775 high.  The walls form teeth for a wave guide.  I’m using opti rough to take the cavity down to .020” remaining, then a swarf mill operation to finish the walls.  The problem is, the simulation shows the part to be perfect, but the physical part is over cut by .005.  I have a +\- .0005 tolerance and I can’t figure out how what’s wrong.  Anyone have any suggestions?

- What kind of machine, control, and setup?

- What kind of temperature control are you using?

- What is the overall size of the part?

- What size and type of Tool are you using, and what kind of Tool Holder?

- Are you using High Speed Machining codes?

- Are you using Filtering on the Toolpaths?

- What is your Tolerance on the physical geometry? (Analyze at 0.000001" precision)

At Methods Machine Tool, we have a Precision Laboratory, with some of the most accurate machines in the world. We routinely hold tolerances much tighter than what you are attempting. I would put this on our Yasda YMC 650+RT20 table. 

Share this post


Link to post
Share on other sites

Collin,

it’s a Robodrill, 5 axis , with a Fanuc control.  Temp is about 72deg.

im using a .047 flat end mill. With shrink fit holding from pioneer.

code is 5axis, G68.2

I’m not filtering, and the total tolerance is +\_.001”.

 

overall size of the part is about 2x3x.5”  

 

and we bought the machine from Methods coincidentaly.

 

  • Haha 1

Share this post


Link to post
Share on other sites

it's a bit late now, but I would have made a test run before the final cut,  with 0.005" stock to leave , measured that it's leaving the 0.005"

and then cut based on the  outcome of the measurement. This comes up very often when I have to make holes for calendar inserts in molds.

for a hole of D6-8 mm and depth f 12 mm if I leave .01 mm even if I hammer the insert in it wont go down all the way. Overcut it by 0.005 mm

and it falls out. So i make a test cut with a step of 0.005 mm  and measure it as the hole grows. I usually get it down to 3-4 cuts altogether.

Gracjan

PS . I suspect your tool was not in the center , or you had a chip between  the tool and the spindle. I just had a case like that a few months ago.

No simulation will help here.

  • Like 3

Share this post


Link to post
Share on other sites

There are a multitude of variables that don't necessarily show up in simulation that influence the end result.

Toolpath Tolerance, Wear comp, filter, tool runout, tool wear, high speed mode active/inactive, etc...

  • Like 2

Share this post


Link to post
Share on other sites
18 hours ago, [email protected] said:

Collin,

it’s a Robodrill, 5 axis , with a Fanuc control.  Temp is about 72deg.

im using a .047 flat end mill. With shrink fit holding from pioneer.

code is 5axis, G68.2

I’m not filtering, and the total tolerance is +\_.001”.

 

overall size of the part is about 2x3x.5”  

 

and we bought the machine from Methods coincidentaly.

 

Hi Keith,

As others in the thread have mentioned; this is likely several different errors combined.

The real key to getting 5-Axis codes like G68.2 to work, is 'fresh calibration', where you are calibrating the following (in order):

  1. Tool Probe (Laser or sensor) > Calibrate the tool measuring device to 1 Micron (0.00004") or better tolerance. (Be as precise as you can, especially if converting from Metric to Inch.)
  2. Spindle Probe Length > Calibrate the Spindle Probe length (to 1 Micron or better). (Calibrates 'Z' measuring accuracy.)
  3. Spindle Probe Diameter > Calibrate the XY of the Probe, using a qualified Ring Gauge. (Class X or better. I prefer Class XX)

After you have calibrated the 'Probing System' (all components, in the correct order), the final 'machine calibration' step is to run the routine to find 'Kinematic Center'. For Renishaw; this would be Axis-Set, and for Blum; Kinematic Perfect.

When running each of these calibration steps, it is critical that you open the 'Settings Macro Programs' (depends on which calibration step you are performing), to make sure the numbers which are 'Hard Coded' in the Settings Macro accurately reflect the real world values. (as accurately as you can.)

Even after performing all of these calibration steps, you still must take into account the following:

  • Mechanical Accuracy > the positioning accuracy and 'repeatability' of any mechanical system will change, depending on the 'loading' of the fixture and part being moved around. Each type of Rotary Table has different specifications for both backlash and positioning accuracy. A table which is designed for 'speed', will always have to sacrifice some accuracy to obtain that speed.
  • Clamping Forces > G68.2 is 'Tilted Work Plane', which is a 3+2 method of cutting. This means that typically you are going to 'position, clamp, then cut'. Actuating the brake to clamp the rotary will typically add a bit to the positioning error. This can often be compensated on the machine by performing 'semi-finish' cuts, measuring the cutting results, and tweaking the Wear Offsets for Length and Radius. However, you now get into the situation where you will need to 'compensate each clamping position'.
  • Tilted Work Plane > Because you are using G68.2, you have the ability to use 'Cutter Compensation' (2D Cutter Comp), and 'Tool Length Offset' (G43). But it also means you will typically need to 'tweak each feature', by either adjusting position (Edit XYZ Position on G68.2 Call), or by using a different 'TLO' and 'CRC' number for each feature. So maybe you've got "T8", and you decide to use 'D81', 'D82', & 'D83', to control 3 separate features, each being cut with the same tool.
  • Semi-Finish Cuts > You should be leaving enough material that you can perform a Semi-Finish Cut (maybe 2 or 3 cuts), so that you can gauge the cutting performance of your finish tool, and find the correct 'Wear Offset Value', so your endmill is cutting 'on size'. I will sometimes take an area of material (in a pocket, for example), which is going to be roughed away, and will start by milling a 'Square boss' in the cavity, and will then perform a series of 'semi-finish' and 'finish' cuts, using the Spindle Probe to qualify the offset. This allows me to 'sneak up' on the correct offset, and qualify the finish tools. I can then rough away all the material in the cavity, and my finish tools are adjusted to cut 'on size'.

 

 

  • Like 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us