Operator Error - What went wrong
Moderator: cnckeith
-
- Posts: 380
- Joined: Tue Oct 20, 2020 8:41 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: Arizona
Operator Error - What went wrong
I just started machining my very first part. I followed the steps to CAM this part from an Online CAM class (Titan CNC Acadamy).
I touched off the on the left and rear of the part with a manual edge finder to set part zero. I set the Z-height using the master tool. I tested my part zero location by entering MDI command and the center of the tool aligned perfectly with the back and left edge of the stock.
When I started running the part, the good news is that the dept of cut was spot on! The intended tool path runs the perimeter of the part and is supposed to remove .050 from all sides. This did not happen.
The tool began running down the left side of the part and just barely glanced the left side taking off almost no material (See images below).
As it ran across the back of the part it removed about .192. It then removed about .093 from the right side.
When it traversed the front of the part, no material was removed as the tool cleared the edge of the part by about .112
I have attached the NC file and put a link to the Fusion file below. One question. When I setup Fusion 360 to cam this part, I had a hard time setting up the correct machine. I ended up modifying a preset Tormach 1100M and selected Centroid as the post. Could this be causing the problem?
Thanks.... Richard
Fusion 360 File:
https://www.dropbox.com/s/4pellf4clkvmr ... 0.f3z?dl=0
I touched off the on the left and rear of the part with a manual edge finder to set part zero. I set the Z-height using the master tool. I tested my part zero location by entering MDI command and the center of the tool aligned perfectly with the back and left edge of the stock.
When I started running the part, the good news is that the dept of cut was spot on! The intended tool path runs the perimeter of the part and is supposed to remove .050 from all sides. This did not happen.
The tool began running down the left side of the part and just barely glanced the left side taking off almost no material (See images below).
As it ran across the back of the part it removed about .192. It then removed about .093 from the right side.
When it traversed the front of the part, no material was removed as the tool cleared the edge of the part by about .112
I have attached the NC file and put a link to the Fusion file below. One question. When I setup Fusion 360 to cam this part, I had a hard time setting up the correct machine. I ended up modifying a preset Tormach 1100M and selected Centroid as the post. Could this be causing the problem?
Thanks.... Richard
Fusion 360 File:
https://www.dropbox.com/s/4pellf4clkvmr ... 0.f3z?dl=0
- Attachments
-
- Titan 1M T2 Adaptive1 12 9 22.nc
- (218.99 KiB) Downloaded 2 times
-
- Posts: 2029
- Joined: Thu Sep 23, 2021 3:49 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: 6433DB0446C1-08115074
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: Germany
Re: Operator Error - What went wrong
What type of manual edge finder?
Did you consider the diameter of the edge finder when setting XY zero?
Uwe
Did you consider the diameter of the edge finder when setting XY zero?
Uwe
-
- Posts: 380
- Joined: Tue Oct 20, 2020 8:41 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: Arizona
Re: Operator Error - What went wrong
Yes, I considered the diameter (.20) and it is a Mitutoyo.
-
- Posts: 2029
- Joined: Thu Sep 23, 2021 3:49 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: 6433DB0446C1-08115074
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: Germany
Re: Operator Error - What went wrong
Did you set zero in fusion to the edge of the stock or model?
Cutter compensation in fusion?
Uwe
Cutter compensation in fusion?
Uwe
-
- Posts: 380
- Joined: Tue Oct 20, 2020 8:41 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: Arizona
Re: Operator Error - What went wrong
I set zero to the edge of the stock. I do not believe cutter comp applies to adaptive tool paths. I did set cutter comp for the other operations. The strange thing is that if it were a cutter comp issue or I had set the edge to model vs stock, I would think the error would be equal on all sides. In this case it removed .192 and .093 from the rear and right side respectively.
When I enter MDI commands, I can make the tool traverse the part correctly. I am thinking that this error has is based upon a Fusion setting. I just have to figure out which setting.
Richard
When I enter MDI commands, I can make the tool traverse the part correctly. I am thinking that this error has is based upon a Fusion setting. I just have to figure out which setting.
Richard
-
- Posts: 2029
- Joined: Thu Sep 23, 2021 3:49 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: 6433DB0446C1-08115074
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: Germany
Re: Operator Error - What went wrong
Adaptive works only with comp in fusion.
Tool Diameter must match with tool in fusion and tool used.
If 0 is set correctly, it is hit and run with swissi PP
Uwe
Tool Diameter must match with tool in fusion and tool used.
If 0 is set correctly, it is hit and run with swissi PP
Uwe
-
- Posts: 380
- Joined: Tue Oct 20, 2020 8:41 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: Arizona
Re: Operator Error - What went wrong
I did set the tool path in CNC12 to match that of Fusion.
When I ran the toolpath originally, I realized that I forgot to turn off Wi-Fi. Not sure if this caused a communication error (I attached the latest report file). I ran it again this morning with the tool height set just .25 inches above the part AND Wi-Fi off.
Totally different results.
The tool path appeared to take no material off the left side of the part
.05 off the rear ... perfect
About .093 off the right
.05 off the front.
I am not sure I understand your cutter comp note. My Contour and Pocket toolpaths are set to LEFT in the passes tab. This option is not available for the Adaptive toolpath. I have it set to CLIMB.
Thanks... Richard
When I ran the toolpath originally, I realized that I forgot to turn off Wi-Fi. Not sure if this caused a communication error (I attached the latest report file). I ran it again this morning with the tool height set just .25 inches above the part AND Wi-Fi off.
Totally different results.
The tool path appeared to take no material off the left side of the part
.05 off the rear ... perfect
About .093 off the right
.05 off the front.
I am not sure I understand your cutter comp note. My Contour and Pocket toolpaths are set to LEFT in the passes tab. This option is not available for the Adaptive toolpath. I have it set to CLIMB.
Thanks... Richard
- Attachments
-
- report_E415F6F649F8-0121214266_2022-12-10_09-36-39.zip
- (883.16 KiB) Not downloaded yet
-
- Posts: 380
- Joined: Tue Oct 20, 2020 8:41 pm
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: No
- Oak CNC controller: No
- CNC Control System Serial Number: none
- DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: Arizona
Re: Operator Error - What went wrong
I forgot to mention. I went back and checked my part zero value for x and ran the part again. Same results.
Re: Operator Error - What went wrong
Use the F8/Graph screen to see what your CNC program really tells the machine to do. You can use pan and zoom controls to read accurate dimensions from the F8/Graph screen, using the rulers across the left and bottom.
In the case of the program you posted at the beginning of this thread, the perimeter cut is a rounded rectangle, with the cutter centerline at:
Left: X-0.1975
Right: X4.0975
Back: Y+0.1975
Front: Y-2.0975
I don't immediately see where you said what your intended part dimensions or boundaries were; or what your cutter diameter is; or what your stock dimensions are, except to imply that the stock was 0.100" larger in X and Y than the finished part was expected to be.
However, speculating that you expected the finished part to be 4" wide and 2" across, using a 0.295" diameter cutter (0.1475" radius); that the stock is 4.1" wide and 2.1" across; and that you intend to set part zero at the back left corner of that stock; then the CNC program is wrong: instead of having the center of the rectangular toolpath at X2.05 Y-1.05 (the center of the stock), the CNC program has a rectangular toolpath centered on X1.95 Y-0.95. That suggests something went wrong in applying your 0.050" shift from the part corner to the stock corner.
Personally, I prefer to set part zero to a corner or feature on the finished part; then -- if I am locating the corner of the stock -- add the cut allowance in the part setup operation. For example, in a part like yours, I would program it to cut around a X2.0 Y-1.0 center, with the corner of the finished part at X0 Y0, and then I would set the back left corner of the stock to X-0.05 Y+0.05.
In the case of the program you posted at the beginning of this thread, the perimeter cut is a rounded rectangle, with the cutter centerline at:
Left: X-0.1975
Right: X4.0975
Back: Y+0.1975
Front: Y-2.0975
I don't immediately see where you said what your intended part dimensions or boundaries were; or what your cutter diameter is; or what your stock dimensions are, except to imply that the stock was 0.100" larger in X and Y than the finished part was expected to be.
However, speculating that you expected the finished part to be 4" wide and 2" across, using a 0.295" diameter cutter (0.1475" radius); that the stock is 4.1" wide and 2.1" across; and that you intend to set part zero at the back left corner of that stock; then the CNC program is wrong: instead of having the center of the rectangular toolpath at X2.05 Y-1.05 (the center of the stock), the CNC program has a rectangular toolpath centered on X1.95 Y-0.95. That suggests something went wrong in applying your 0.050" shift from the part corner to the stock corner.
Personally, I prefer to set part zero to a corner or feature on the finished part; then -- if I am locating the corner of the stock -- add the cut allowance in the part setup operation. For example, in a part like yours, I would program it to cut around a X2.0 Y-1.0 center, with the corner of the finished part at X0 Y0, and then I would set the back left corner of the stock to X-0.05 Y+0.05.
-
- Posts: 3110
- Joined: Tue Mar 22, 2016 10:03 am
- Acorn CNC Controller: Yes
- Allin1DC CNC Controller: Yes
- Oak CNC controller: Yes
- CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192 - DC3IOB: No
- CNC12: Yes
- CNC11: No
- CPU10 or CPU7: No
- Location: Boston, MA
- Contact:
Re: Operator Error - What went wrong
When I work from rough stock, I always use the center of the part. This ensures equal amounts are taken off all sides.
Cheers,
Tom
Confidence is the feeling you have before you fully understand the situation.
I have CDO. It's like OCD, but the letters are where they should be.
Tom
Confidence is the feeling you have before you fully understand the situation.
I have CDO. It's like OCD, but the letters are where they should be.