Rotate/Translate Axes?

[jim_stoll]

I've got a Partmaster Drawing (.dra) and resulting Machining (.cnc) file that is oriented with the standard XYZ axes. I mounted my chunk-o-metal all firmly to my table, got it all squared up w/ the mill axes and discovered (thankfully before attempting to cut), that I have it mounted 90 degrees off. Positive X in my drawing needs to be negative Y on my setup, and positive Y in my drawing needs to be positve X on my setup. (I did manage not to bungle the Z... :-)

Is there a simple way to translate axes so that this type of situation can be handled? (BTW, I'm using PartMaster v8, if that makes a difference.)

Thanks Much!

[jim_stoll]

Update - I selected all elements in the drawing and rotated the whole set by 90 degrees, then shifted it down into the +x/-y quadrant. I'd had the 'bottom' of the part originally lying on the X axis, with the left most edge of the part against the Y axis. After the rotation/translation, the former left edge was against the X axis, while the former 'bottom' of the part was lying along the negative Y axis. I re-imported it into DCAM and Post Processed it and got an interesting result.

There was a 3/8" hole in the middle of the part, constructed of 4 G03 commands (by PartMaster):

G03 X1.4 Y0.5438 I-0.0938 J0.0
G03 X1.3063 Y0.45 I0.0 J-0.0938
G03 X1.4 Y0.3563 I0.0938 J0.0
G03 X1.4938 Y0.45 I0.0 J0.0938

and this processed fine when the part was in its original position. But, in the new position, I got an incomplete G03 command after the 4 arcs constructing the hole:

G03 X0.545 Y-1.3996 I-0.0001 J0.0938
G03 X0.4513 Y-1.3059 I-0.0938 J0.0
G03 X0.3575 Y-1.3996 I0.0 J-0.0938
G03 X0.4513 Y-1.4934 I0.0938 J0.0
G03 I0.0 J0.0938

and EMC complained, rightfully so. The hole was 1" deep, so was made by 4 .25" deep passes, and each of the 4 passes had this extra, incomplete G03 command.

Any thoughts/ideas on why this happened? I simply removed the 5th G03 from each of the circular passes and the was palatable to and ran fine in EMC. If I can avoid this happening at all in the future though, that would be preferrable. (Chad, if you're reading this, this was using the Post you recently modified for me, though I got the same results using the original, unmodified M_TurboCNC_Triac.ppr Post as well.)


Thanks Again!

[Chad_Clark]

This is a tolerance problem, it can be fixed quite easily with a small mod to the post-processor.

What version of PartMaster do you have - when is it dated ? There has been changes recently (to V9 and V10) affecting arc splitting.

If I can get a copy of the .cnc file I can test exactly what is happening and decide the best course of action.

[jim_stoll]

Hi Chad,
I'm using Dolphin Partmaster Milling and Turning module Version 8, 2, 1004. I couldn't find any file date in the About window, but the file date on the Dcam.exe file is 3/2/2004.

I'm attaching the .cnc file that is resulting in the extra G03 command. The tool being used is a .1875 IN endmill. Below is the generated gcode. This is from the TurboCNC Post that you just recently modified for me. (I renamed the file to differentiate it from the prior version.)

%
( Produced :- 22:52:03 Monday, September 17, 2007 )
( CNC File :- ExtraG03Hole )
( Post Processor :- M_TurboCNC_Triac3 )
G90
G20
G00 X0.0 Y0.0 Z0.25
G00
M05
M06 T03 ( End Mill )
M03 S1000
M07
M03 S1000
G00 X0.4513 Y-1.4934
G00 Z0.1181
G01 Z-0.25 F0.163
G03 X0.545 Y-1.3996 I-0.0001 J0.0938
G03 X0.4513 Y-1.3059 I-0.0938 J0.0
G03 X0.3575 Y-1.3996 I0.0 J-0.0938
G03 X0.4513 Y-1.4934 I0.0938 J0.0
G03 I0.0 J0.0938
G00 Z0.25
M02
%

As always, Thanks a Bunch!!

Jim

[jim_stoll]

Also, so as not to lose track of my original question on this... Is there a means of translating axes in the CAM module? I'm guessing that there must be plenty of cases in the real world that through choice or error, material is fixtured in a way that does not correspond to the original drawing's axes. Can this type of situation be dealt with in Partmaster w/o having to go back to the original drawing to translate all of the components manually?

Thanks Again!

[Chad_Clark]

I have checked the V8.4.1018 (which is the earliest I can find) source code and compared it to the V9 code. There is a bug in V8 which can cause a spurious arc move to be output. It is caused by tolerance errors when splitting arcs at quadrant boundaries - as required by some controllers. If the arc ends very close to a quadrant boundary (i.e. more than 0.000004" from the quadrant boundary) there is a 50% chance of an an errant arc move being output.

This problem was fixed in version 9, now arcs which end very close to quadrant boundaries (ie within about 0.0003" of the quadrant boundary) are treated as if they end exactly at the quadrant boundary. This eliminates the spurious arc block.

DCam V9 and V10 both support axis scaling, translation, rotation and mirroring.

You would need to upgrade at least to V9 (and preferably V10) to fix the arc problem.

There has been numerous improvements and bug fixes since V8.2.1004. There will be no loss of functionality, and a host of new features assuming the customer opts for Level 3. (There was no concept of L1, L2 or L3 in Version 8, there was just the standard version and a Mach2 version which would only run the Mach post processors.)

Many of the NC code generation routines have been completely re-written to produce more efficient toolpaths - especially in turning.

[Chad_Clark]

Originally Posted by jim_stoll Also, so as not to lose track of my original question on this... Is there a means of translating axes in the CAM module? I'm guessing that there must be plenty of cases in the real world that through choice or error, material is fixtured in a way that does not correspond to the original drawing's axes. Can this type of situation be dealt with in Partmaster w/o having to go back to the original drawing to translate all of the components manually? Thanks Again!

Jim,

Not in the verison that you are using, but in V10, it will incorporate axis translation and rotation in the fixture offset.

[GSSTUART]

Chad- Could you please give more direction about fixture offset in V10.
I tried it and it asked for an offset register, is this something that I have to define in the ppr? Also I didn't see any options for rotation, only translation.

Thanks
Gary

[Chad_Clark]

The fixture offset feature (Setup menu > Fixture offsets) is intended to allow the user to assign geometry (Contours and Patterns) to various named groups. Each group has associated with it a local datum point and a fixture offset number (in the range 1 - 6).

If this facility is used then any machining applied to a contour/pattern which is in a fixture offset group is translated to the group's local datum point.

If the post-processor is setup to use fixture offsets (typically G54 through G58 and G59 which cancels the offset) then the post will output the relevant Gcode. The XYZ data is output unmodified.

If the post-processor is not set up to use fixture offsets, it will modify XYZ data by adding on the XYZ value of the fixture offset group local datum.

Either way the end result is the same, machining is offset relative to the machine zero.

Since most older controllers do not support axis rotation as part of their fixture offset capabilities it is not implemented here - but may be in a future release.

To cope with combined translation and rotation, use the Repeat machining command.
Set Repeat to 1 in X and 1 in Y, now you can use the Mirror / Scale / Rotate / translate tabs to mimic "fixture offset" in a way that does not depend on any of the machine controller capabilities.

You must use the repeat commands in pairs, the first one switches on, the second switches off. All machining in between them is affected by the parameters specified by the first Repeat command of the pair.

I have sent a .CNC file to your email so that you can see the set-up and example. Just save it to your computer and then open it with the Partmaster CAM program by choosing open existing job. I hope this helps

[GSSTUART]

Thanks Chad - That will definitely come in handy. One additional question. When I tried the repeat sequence on a file of mine that is in inch units the rotate and translate fields were in mm. Do I just do the math or is there a global units switch that I have not set.

Gary

[Chad_Clark]

Originally Posted by GSSTUART Thanks Chad - That will definitely come in handy. One additional question. When I tried the repeat sequence on a file of mine that is in inch units the rotate and translate fields were in mm. Do I just do the math or is there a global units switch that I have not set. Gary

Gary,

They should be in inches (0.0"). As long as your machine set-up is set in inches.

Chad