Operator Error - What went wrong

A place to discuss and ask questions about all things Machining for Mills, Lathes, Laser, and Routers

Moderator: cnckeith

RJS100
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

Post by RJS100 »

Thanks for your detailed review of the g-code and idea of using the graph function. I never realized that the graph had a scale. Nice!

For now, I am doing my best to closely follow this online course to cad and cam 10 fundamental parts to help learn the process. The attached image shows the part/model setup in Fusion. I followed the lesson to a "T" with just a few changes:

1. The course created a part that is 2" x 4" with the stock being oversized by .1 inches. I happen to have a piece of stock that was 2" x 4" so I reduced the size of the model to 1.9" x 3.9".

2. I changed the speeds & feeds commensurate with my machine. Uwe reviewed the speed and feeds and thought they were good to go.

The code that you reviewed is for an Adaptive toolpath using tool #2 (3/8" carbide end mill).

You noted:
Left: X-0.1975
Right: X4.0975
Back: Y+0.1975
Front: Y-2.0975

This toolpath traversed with a 3/8" end mill would create a rectangle that is 1.92" x 3.92" This is very close to the intended size of 1.90" x 3.90". When I graphed this with CNC12, I got the same 1.92" x 3.92". I have no idea as to why the size is off by .020 inches.

Thanks for helping me establish that the tool path is oversized a bit and appears to be shifted to the right.

The only thing I can think of is that I setup a machine in Fusion 360 by using a stock machine (Tormach 1100) and modified it to look like my PM-833TV. This machine may have some translations that I am not aware of. My next step is to delete the machine in Fusion, and then post the nc code using the Centroid post. I can't think of anything else to try.

Richard
Attachments
Part Zero.JPG
tblough
Posts: 3071
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

Post by tblough »

From the image, the part origin is on the corner of the part, but you said earlier you were setting your WCS on the corner of the stock. That is why it is cutting twice as much on the right side and front, and barely cutting the left end and back

The reason the program is cutting 1.92 and 3.92 is you probably have a 0.010" finish cut. That will take 0.01" more off all sides leaving 1.9 x 3.9.
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.
suntravel
Posts: 1967
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

Post by suntravel »

0 in fusion was set to model, not stock, if you do so you must set 0 with the stock offset in Acorn.

I have set it to the edge of the stock, but consider using the middle of the part as Tom suggests.

Install swissis post, that is the best on for milling with Acorn.

I have attached g-code posted with swissis PP.

Uwe
Attachments
1001.zip
(75 KiB) Downloaded 2 times
fu03.jpg
fu02.jpg
fu01.jpg
RJS100
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

Post by RJS100 »

Guys... Thank so much for all your help. I knew that this was a case of operator error. Yes, when I touched off the part, I totally forgot to jog inbound .050 for x and y axis. I downloaded the Swissi PP from git hub (I hope I got the latest version, see below). I then re-established part zero location for x and y and everything worked great! Attached is an image of my first part with an adaptive tool path. I also found out that the coupling on my y axis stepper was not tight enough and was slipping. All good now!

Thanks so much for all your help!

Quick question. When I ran this the 1st time with the wrong part zero, the cutter made a cut that was .17 wide and .36 deep across the back of the part in one pass. I was running at 3000 rpm and 10 ipm. The tool was .375 diameter three flute carbide end mill that has 1.25" of stick out. I was surprised that it seemed to make this cut effortlessly. For fun I plugged these figures into the G-Wizard calculator (see below), and they appear to be less aggressive than I thought. What do you think, is this an aggressive cut for a 2HP benchtop machine?

Thanks... Richard
Attachments
G Wizard.JPG
20221211_172522.jpg
Swissi.JPG
RJS100
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

Post by RJS100 »

Hello Uwe,

I finished the rest of the toolpaths for my 1st part, and they all worked great! Thanks for your help getting started. One last question, I was reviewing the documentation for Rigid Tapping so I can finish this part with tapped M4 holes. I noticed that the documentation recommends tapping at 640 rpm.

If I understood you last comment, you suggested tapping these holes at 2000 rpm. Is there something else I should be considering?

Richard
Attachments
Part.png
suntravel
Posts: 1967
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

Post by suntravel »

You can start with 640 rpm. 2000 works for me because my spindle servo is fast with direction change.

For first setup I do airtapping over the part, if it looks ok go deeper or change parameters.

Good test is also to tap a piece of wax,

Uwe
tblough
Posts: 3071
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

Post by tblough »

Centroid recommends 640 because that is the speed suggested when setting up rigid tapping. There are quite a few variables that control the tapping process and are all affected by spindle inertia.

If you use a different speed, you may have to adjust the rigid tapping parameters accordingly.

Machinable wax is recommended for setting up rigid tapping as Uwe mentions. It is very forgiving and will not break taps or damage the machine if you've made a programming mistake. At the same time, it is very brittle and setup errors can be easily seen in the finished threads.
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.
RJS100
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

Post by RJS100 »

Thanks... Looks like I will go order myself some machinable wax.

Have a great weekend... Richard
suntravel
Posts: 1967
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

Post by suntravel »

RJS100 wrote: Sun Dec 18, 2022 2:33 pm Thanks... Looks like I will go order myself some machinable wax.

Have a great weekend... Richard
I must admit that I never used wax :D

I use a ~1/4" piece aluminum, drill an array of trough holes, airtap over the holes, tune parameters, go deeper and fine tune.

Even with going to fast on the ramps and get a spindle error, never broke a tap. Z is tied very well to the encoder counts.

But consider the tap will go a little deeper than programmed, because of deceleration. So be careful with blind holes.

If not deep enough, you can tap a second time deeper, if to deep a small tap will break.

Uwe
RJS100
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

Post by RJS100 »

Thanks.
Post Reply