Keyboard Shortcuts
ctrl + shift + ? :
Show all keyboard shortcuts
ctrl + g :
Navigate to a group
ctrl + shift + f :
Find
ctrl + / :
Quick actions
esc to dismiss
Likes
- MachCNC
- Messages
Search
|
Locked
Re: arc question
开云体育i made the holes with cambam and it did what it did. i would much
prefer a single arc but i thought they had to be less than 180
degrees or some other limit. i just trusted what canbam made. i like the idea of parameters i use them all? the time in
computer programming. i think i should start over with the two holes and learn how to
specify a single arc or find a program that does instead of three
or four. Will Estlcam do this? On 2/14/2022 2:41 AM, Martin Connelly
wrote:
-- Best regards, Spencer Chase 67550 Bell Springs Rd. Garberville, CA 95542 Postal service only. Laytonville, CA 95454 UPS only. Spencer@... (425) 791-0309 |
|
Locked
Re: arc question
I will try to do it this way. I wanted to use cutter comp but could not figure out how to do it with I J specs. It sort of seemed impossible.
toggle quoted message
Show quoted text
Will Mill Wizard make simple easy to understand gcode for holes? I have made much more complicated with cambam but for flat pieces. this part has three machined faces 90 degrees apart and i figured i would never get the positions right so i made all the features centered around 0 and then used offsets to get them right. The problem is that if i halt the program and rewind it the offsets can be left a mess and i have to restart Mwch4. Just homing and 0 ing offsets does not always work. If there is a way to completely remove all offsets (including ones that appear to be hidden?) that would allow me to keep the confusing but editable code as it works quite well. When doing a circle with Mach 4 in several arcs aren't they just as smooth if the speed does not change and trajectory planning is left on? I did not notice hesitation at the move from arc to arc? On 2/14/2022 3:53 AM, Brian Barker wrote:
If your willing to do 180 or less you can do R style arcs. I find that most people have a hard time with the I J vectors to tell where the start point is. But the radius seems to be something that everyone can do ! --
Best regards, Spencer Chase 67550 Bell Springs Rd. Garberville, CA 95542 Postal service only. Laytonville, CA 95454 UPS only. Spencer@... (425) 791-0309 |
|
Locked
Re: arc question
If your willing to do 180 or less you can do R style arcs. I find that most people have a hard time with the I J vectors to tell where the start point is. But the radius seems to be something that everyone can do !
toggle quoted message
Show quoted text
G0 X1 Y1 G02 X2 R.5 F50 G01 Y0 G02 X1 R.5 F50 G01 Y1 M30 This is how I do it when I am doing hand coded parts. I also use cutter comp so I can reuse the code for finish and roughing passes. But I have been told that I am not normal anymore :( Thanks Brian ______________________________ Brian Barker Engineering / Development ArtSoft | Newfangled Solutions Livermore Falls, Maine (USA) Webpage: On 2/13/2022 2:09 PM, spencer@... wrote:
that is the first place i looked. i did a couple of tests but not a successful one yet. the one in the thumb drive that i have not tested yet should work. i probably got some addition wrong in the first one. i need to figure out how to use my calculator reliably with negative numbers. Actually I just thought of using a spreadsheet but the copying and pasting would be a bitch. |
|
Locked
Re: arc question
Have you got CAD in any form? Can it export a DXF file? If you have answered yes to both of these it may be worth using a simple DXF to Gcode CAM program to create your Gcode. The one I use is Estlcam. This is available for download and can be used a number of times before you get a nagging to buy it. It takes a small amount of time to be able to use it easily but it is worth spending some time with it for relatively simple jobs like this.
I also do not understand why the circular path has been divided into three segments when a single line of code can replace the three arcs you have used. G52 X 0.01 Y .6125 (thru hole) (1ST PASS) G1 F146 X0.0095 Y0.0 G1 F52 Z-0.34 X0.2095 G2 F40.0 X0.2095 y0 I-0.2095 J0.0 This makes it easier to understand and to change to climb milling you just need to change the G2 to G3 Another option is to arc into the start position by changing the line?G1 F52 Z-0.34 X0.2095 to G2 F40 Z-0.34 X0.2095 I0.1 J0 This could all be followed by an arc out as well G2 F40 Z0 X0.0095 I-0.1 J0 G52 X 0.01 Y .6125 (thru hole) (1ST PASS) G1 F14 X0.0095 Y0.0 G2 F40 Z-0.34 X0.2095 I0.1 J0 G2 F40.0 X0.2095 y0 I-0.2095 J0.0 G2 F40 Z0 X0.0095 I-0.1 J0 The arc in and arc out avoids dwell at the start and finish of the hole to keep it smooth Have you considered using parameters to produce your gcode? For a simple hole like this you can have four parameters such as #51, #52, #53 #54 which are used for the hole position X, Y, the depth Z and the radius of the path. For your hole for example (thru hole)
?
#51 = 0.0095? ? ?(X position)
#52 = 0? ? ? ? ? ? ? (Y position)
#53 = -0.34? ? ? ? (Z depth)
#54 = 0.2095? ? ?(radius)
?
(1ST PASS)
G1 F14 X#51 Y#52 Z0
G2 F40 Z#53 X[#51+#54] I[#54/2] J0
G2 F40 X[#51+#54] y#52 I[0-#54] J0
G2 F40 Z0 X#51 I[0-#54/2] J0
Change the #number parameter values to suit your needs. You can repeat the section as many times as needed with different parameters? to make a pattern of holes and differing depths and diameters as well. You could also another parameter for the initial Z height. ?
Martin |
|
Locked
Re: arc question
that is the first place i looked. i did a couple of tests but not a successful one yet. the one in the thumb drive that i have not tested yet should work. i probably got some addition wrong in the first one. i need to figure out how to use my calculator reliably with negative numbers. Actually I just thought of using a spreadsheet but the copying and pasting would be a bitch.
toggle quoted message
Show quoted text
Then I thought of writing a script to apply the offsets but that would be pretty complicated and a lot of work for one use. Does anyone have a script already written to do this? If I clean up the gcode, remove comments format every statement the same, it might not be too difficult of a script. i am just so awful at simple math. i would rather figure out a complicated formula than add a couple of numbers :) And don't ask me about multiplying. I would be lost without a calculator. i am working on the spreadsheet, decided scripts will take all day to write. On 2/13/2022 2:13 AM, Paul Galarneau via groups.io wrote:
Take a look at this web page, very clear: --
Best regards, Spencer Chase 67550 Bell Springs Rd. Garberville, CA 95542 Postal service only. Laytonville, CA 95454 UPS only. Spencer@... (425) 791-0309 |
|
Locked
Re: arc question
Take a look at this web page, very clear:
toggle quoted message
Show quoted text
:) :) -----Original Message-----
From: [email protected] [mailto:[email protected]] On Behalf Of spencer@... Sent: Saturday, February 12, 2022 8:12 PM To: [email protected] Subject: Re: [MachCNC] arc question To answer my own question maybe. It looks like I am j are relatibe so they should not be offset Feb 12, 2022 4:02:44 PM spencer@...: I have some gcode that I wrote a long time ago, using cambam, I think. Itmade the circles for me so I did not need to understand G code arcs. Over the years I have move the circular pockets relative to each other by using offsets. on arcs but is moving the location of an arc less complicated than I think it may be? Here is an example. I use G52 to set the X and Y offsets. To move the circle without using offsets do I just need to add the offsets to all X and Y coordinates and add the X offset to the I and the Y offset to the J.
|
|
Locked
Re: arc question
To answer my own question maybe. It looks like I am j are relatibe so they should not be offset
toggle quoted message
Show quoted text
Feb 12, 2022 4:02:44 PM spencer@...: I have some gcode that I wrote a long time ago, using cambam, I think. It made the circles for me so I did not need to understand G code arcs. Over the years I have move the circular pockets relative to each other by using offsets. |
|
Locked
arc question
I have some gcode that I wrote a long time ago, using cambam, I think. It made the circles for me so I did not need to understand G code arcs. Over the years I have move the circular pockets relative to each other by using offsets.
I want to get rid of the offsets for various reasons. I still am not clear on arcs but is moving the location of an arc less complicated than I think it may be? Here is an example. I use G52 to set the X and Y offsets. To move the circle without using offsets do I just need to add the offsets to all X and Y coordinates and add the X offset to the I and the Y offset to the J. I hope it is that easy :) G52 X 0.01 Y .6125 (thru hole) (1ST PASS) G1 F146 X0.0095 Y0.0 G1 F52 Z-0.34 X0.2095 G2 F40.0 X-0.1048 Y-0.1814 I-0.2095 J0.0 G2 F40 Y0.1814 I0.1048 J0.1814 G2 X0.2095 Y0.0 I0.1048 J-0.1814 -- Best regards, Spencer Chase 67550 Bell Springs Rd. Garberville, CA 95542 Postal service only. Laytonville, CA 95454 UPS only. Spencer@... (425) 791-0309 |
|
Re: Limit and Home switches
I think if you are using one switch for home and the same switch for limit and you are using a smoothstepper.
then in the smoothstepper config under inputs if homing motor0 and say using motor0 limit ++ or -- then turn them on and use the same pin? under inputs in ESS config. if you are using 2 switch's (home combined with one limit) then you will need a separate pin set for the other switch for limit++ or -- however your direction is setup... ? ? |
|
Re: strange problem and possible solution
开云体育I have tried every speed and feed combination and almost anything works for 90% or more. It is just that less than 1% where I have to reduce the feed to about 40% and it still chatters. I tried to make the motor driver fault when the motor is overloaded and can not do it. The minimum max amps is something like 1.9 amps and holding a wooden stick on the spindle nuts until it burns, the motor does not stall or trip the overcurrent so this is not an option. However I think I finally figured out what the "real" problem is.
The motor has plenty of power and the bit can certainly cut
through almost anything. I have a forth axis to machine three
surfaces of the part. It uses a stepper and a pneumatic that
"locks" the forth axis in place. However is is just a block that
clamps one of the three surfaces of the pneumatic "vise" What is actually happening is that when the bit hits the strange hard uneven end grain instead of cutting it moves the part along the third axis tries to climb the block and just plain fucks up. I had noticed the vise moving along the fourth axis (rotary) but never made the connection that this is the beginning of the serious fuckup. If the fourth axis did not budge the bit would probably roughly chew through the tough grain. So after I get some work done today I am going to make the "lock"
a real lock with a pin instead of just a clamp. However when the
awful chatter happens it is likely to lose steps so I have to re
home the machine but at least I will not break the cutter or run
it into the cylinder on the vise or ??? in the next move. On 2/7/2022 7:19 AM, sdmonaco via
groups.io wrote:
-- Best regards, Spencer Chase 67550 Bell Springs Rd. Garberville, CA 95542 Postal service only. Laytonville, CA 95454 UPS only. Spencer@... (425) 791-0309 |
|
Limit and Home switches
Hi
I have a 3 axis mill developed from a conventional Milldrill with ballscrews and drives added. All working and functioning correctly. As is the home and -ve axis limits. How can I use the home switch as a limit when in normal operation? Or is there settings I have missed? I tried adding the limit with same port and pin number. Howeve this works when running the G28 and stops the homeing from completing. Thanks Graham |
|
Re: strange problem and possible solution
开云体育the motor is more than adequate, i think it is 2 HP wired with a
fairly short proper cable. I should check the connections could
have loosened. I have a big button estop that cuts power to everything but the computer and breakout board and ESS so I am only using the estop on the breakout to not allow the program to run if the motor is not running but this does not work as I would like. I was cautioned to use only NC estop for safety reasons but feel confident that I can us NO as long as I have the mechanical estop. So I am going to change the VFD inverter to? close the relay contacts (unfortunately it only has NO contacts) when it faults or when the motor current overloads. This wood is really strange, almost all of it cuts just fine. But
occasionally when starting into endgrain it provides a lot of
resistance. Again 95% of the time it is fine cutting at fairly
high speed but just occasionally it it a problem. I might also experiment with different speeds for the arcs that
lead into endgrain. All of my circles and D shaped cuts are made
of multiple arcs so this experiment should not be too difficult.
However I have found that in general it is not good to vary the
speed in a series of arcs. Wood is definitely a different beast from metal or plastic. Never
have any of these problems with other materials. On 2/6/2022 5:45 AM, notoneleft wrote:
-- Best regards, Spencer Chase 67550 Bell Springs Rd. Garberville, CA 95542 Postal service only. Laytonville, CA 95454 UPS only. Spencer@... (425) 791-0309 |
|
Re: strange problem and possible solution
开云体育I'd guess it's a spindle issue, unless you are making really deep cuts at high speeds. Other than cutting through a know, no sharp 1/4" tool should have trouble cutting through any wood. How powerful is your spindle?
Ger
On 2/5/2022 5:11 PM,
spencer@... wrote:
I have been having occasional strange behavior making small parts on my |
|
strange problem and possible solution
开云体育I have been having occasional strange behavior making small parts on mycnc router and think I finally figured out what is causing it. I thought it was miss-feeds or just about anything else but have almost certainly determined that there are (fortunately occasional) blocks of wood that are unbelievably hard, almost impossible to cut. I discovered this today and am using a SouthEast tool 1/4" down spiral bit that is almost virgin so it is not the tool. The spindle boggs down and then all hell breaks loose while moving with no cutting action. Or at least I think this is what is happening. quick estopping resetting the machine and starting over confirms that the wood is in fact very difficult to mill. I am using an xbox controller that has plenty of spare buttons so I configured the big 4 way toggle button to be feed hold. I did not want to use feed hold because I thought there was a warning about resuming from feed hold. But I tested it and it seems to work correctly When I get the first indication that a piece of wood is like a stone, I hit the feed hold button on the xbox, set the feed to 40% and hit run again. Then before running the next part I set it back to 100% Wouldn't you know that right after implementing this I ran into a wooden rock and the method worked. It has been years since I set up the VFD spindle controller and I sort of think that I have it halt on overload. Maybe I should turn that feature off and hope it powers through at a slower speed? Seems like a pretty awful idea to me? Any opinions of screwing around with the spindle fault settings? |
Graham
to navigate to use esc to dismiss