603,783 active members*
3,388 visitors online*
Register for free
Login
IndustryArena Forum > CNC Plasma, EDM / Waterjet Machines > Waterjet General Topics > New guy question..Need a where to learn answer
Results 1 to 12 of 12
  1. #1
    Join Date
    Feb 2007
    Posts
    3

    New guy question..Need a where to learn answer

    I have a friend that has built a new table for himself so he could cut his own brackets for what he sells.

    He made it pretty big.
    He has a thc 1000 he has mach 3 and sheetcam and auto cad loaded on the pc that is hooked up..

    I'll keep it simple..
    Where could a shmuck like myself learn how to use those programs..He is an excellant fabricator, but somewhat computer illiterate.
    We both know the computer programing would tick him off the most because he is not familiar with it..

    I would love to jump in and learn these programs so we could start messing with his table..

    Please don't flame me out..
    The most I know is how to make a picture in auto cad. save it as a dxf and pull it up in sheetcam.. But to make the g-code to use in mach 3.. I have no idea.
    i read somewhere about lead in and other things that should be done with sheet cam. But I am stuck there.
    I can open a .tap fil with mach3 but it doesn't move his table and usually reads error with line 8 for gcode..

    If there are books on this or if anyone in the spokane Wa area can hook me up. It would be appreciated.

  2. #2
    Join Date
    Sep 2006
    Posts
    10
    In the sheetcam software there is a "Plasma Tutorial" under the help dropdown menu. Go through the steps in this and it Outputs a basic G Code for your Machine. Make sure you have the right post prossesor selected or it will not output the G code as you need it. I am not a big Autocad supporter. I have found BOBCAD to be easy, economical, and works great for me. Good luck

    Tom

  3. #3
    Join Date
    Oct 2005
    Posts
    1238
    Welcome to CNCzone.

    The Artsoft web site has tutorials for Mach 3.

    Try your local community college, library, or bookstore for Autocad, to help with those "pictures."

  4. #4
    Join Date
    Mar 2006
    Posts
    759
    :wave: Another "welcome to CncZone" here.
    First, you need to define your settings in Sheetcam.
    Set up at least 1 or two tools to use (pulldown menu, goto-tools, new plasma cutter) and enter all the info needed, set up one tool for 1/4 inch plate, for instance. Here is some "generic" tool settings for 1/4 plate. It differs with each plasma, but it is a start.
    Tool -0
    names- plasma 1/4 plate
    kerf-.05
    feed- 45 ipm
    pierce delay-2 sec
    pierce height .188
    plunge-100 in/min
    cut height- .07
    pause at end of cut- 1sec
    Now go to options>select post processor> Mach2 plasma, and hit ok.
    You will need to go to options>material and define the size of the material. I just leave mine on 4'x4'
    now go to options>machine, and make the machine origin the bottom left corner, and tell it how big your machine is in X and Y coordinates. Say 48 inches in Y and 96 inches in X for a 4x8 table.
    Now load a drawing from the file pulldown (upper left corner), you can load drawings or job files, but for now, until you really get the hang of it, just use drawings. Load your DXF files, and it should appear in the bottom left corner of the screen.
    in the bottom left of the screen, you will see a "G" and "V", then a drill bit, and above that, a small torch icon. Click on it, and tell it which tool you want to use, and whether you want inside or outside offset.
    NOTE: if your drawings are not completely connected right (say from a arc to a straight line), the inside/outside offsets will not work right.
    You will have to select which layer the drawing is on, usually Default or 0. If one doesn't work, try the other.
    Now, inside that same box that appeared, click on cut path. Click auto optimize, and all inside cuts first.
    Again, this will get you started. Once you get the hang of it, you can toy with your settings for optimum performance
    Your drawing should now appear in red and green colors. If it shows in white, try a different layer in the previous box.
    This is how your part will be cut. Click on the green "P" at the top of the screen, and you have now made your "G" code.

    Load that in Mach, and make sure you have Mach configured properly.
    need more help, give me a shout.
    Sorry for the long post, but it is as step by step as I could get it.
    Hope this helps!
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    "If the women don't find you handsome, they should at least find you handy"
    -RedGreen show.

  5. #5
    Join Date
    Nov 2005
    Posts
    1468
    After you "Post Processor" it always dry run any G-Code with the Z well away from the part. I've had some rather elegant G-Code plough a turret mill into the actual machine whilst franticaly scrabbling for the E-Stop button and trying to get my head out of the way of the awful noise lol

    I actual fact, what I do with that turret mill now is stick a big black inky pen in the tool holder and turn the spindle off.. run the prog and I can see EXACTLY where the beastly machine sneakily sends the tool hehe.

    [Edit]Oh! and welcome no- one will flame you here for asking these kinds of questions.. they're a nice bunch really... unless they run out of coolant lol[/edit]
    I love deadlines- I like the whooshing sound they make as they fly by.

  6. #6
    Join Date
    Feb 2007
    Posts
    3
    Thanks guys.. This is just something new and big we jumped into with both feet. We are tired of sending out diagrams and measurements to outside sources.

    We came across this site a little while ago and made the decision to go through with this table build..

    I will definately thank all of you in advance and try not to miss any knowledge you guys toss at me..

    We laughed the other day watching american choppers and saw how easy they made it look to cut a piece out of a 5-axis cutter9Wonder how long it took to get to that point), and we can't even get a program to work......

  7. #7
    Join Date
    Jul 2005
    Posts
    2415
    There are three pieces to the equation. The first is the CAD/Drawing part. That will probably be the longest learning curve if you have not done that before. Start with simple objects (circles, rectangles, etc). You will get frustrated and want to throw the whole thing out of the window. Resist the temptation! It will finally start to click and with practice you will be able to draw what you want.

    The second is CAM. That part is easier. The SheetCAM app is pretty straight forward. As stated earlier you need to setup "tools" to cut with. A plasma torch has properties like kerf width, feedrate (cut speed), pierce height, initial cut height, etc). Each type of tip needs to have a different tool setup. You may even want to define different tools for different materials.

    Load the drawing and learn how to use the different "cursors" at the top of the drawing area. Each one allows you to select different actions. The "C" is a Contour cursor that lets you select individual chains of nodes (contours). Think about how you want to cut the job. You want to "group" types of cuts together (inside. outside, online). You do that with Layers in SheetCAM. Select multiple contours using the left mouse button and the CTRL key on the keyboard. Once you have your group selected right click an element and tell it to move it to a "new" layer and then name it something that makes sense to you like "inside detail cuts" or "online cuts".

    Once you have all of the contours assigned to a group then build a list of cut "processes". Select a plasma symbol on the process list (lower left window) and a window comes up that lets you select one of your Layers you named and the tool (remember the list of plasma tools) and HOW you want it cut. (Inside and outside cuts have to be made on "closed" objects). You can set a new feedrate and you can define a lead-in and/or lead out and lead types. For starters use something like a 1/2" lead-in Tangential mode and no lead-out. Once you finish that process the blue cutpath will appear on that Layer (group) of contours along with the lead-ins. It will even show you the offset from the actual drawing.

    Once you have all the processes defined (they cut in the sequence you have them in the list) they can be reordered by dragging a process up or down in the list. Obviously you want to make inside cuts prior to the final outside cut.

    The third piece is the Control.....
    Now is the really neat part: Select the right Post Processor to use (The MP1000 comes with one for SheetCAM on the CD). Then just hit the big "P" at the top of the page and SheetCAM prompts you for what you want to name the g-code file and spits out hundreds or even thousands of lines of g-code in a second.

    Load the g-code into MACH3 and Home your machine and try it with the power to the plasma Torch and the THC Button in MACH turned off.

    Once again start simple. Draw a square and a circle and move them to SheetCAM. Setup the cut processes. Play with inside and outside cuts.
    Generate the g-code and Load it in MACH. Look at the toolpath and if it looks like what you drew then try a dry run.

    When you set your THC feedrates, and tip volts use the tables that come with your plasma torch.

    If you need some more help make sure you are a member of my support site. Other owners of MP1000's hang out there and also use the same tools you want to learn. There are some neat pieces of decorative plasma artwork in the files section of the support site (CANDCNCSUPPORT Yahoo Group). They are in CDR (CorelDraw) native format but scrounge up a copy of CorelDraw 12 and you can open them and use the Free Demo of DXFTools from www.candcnc.com to convert them to perfect DXF files for SHeetCAM.

    TOM CAUDLE
    www.CANDCNC.com

  8. #8
    Join Date
    Feb 2007
    Posts
    3
    Massa and Torch.. Thank you guys for the input..
    Torch/Tom I think My buddy has been in contact with you. Blackbird ring a bell?

    I took your info and sat at his computer
    Here is what happen.

    I input all of what massa gave me except for the post processor. I put what torch said to use for the mp 1000

    I took a dxf which has worked fine for the company we would use to cut our stuff. Well, a couple questions have arose from just palying with this...

    1. all inputs put in like this
    Tool -0
    names- plasma 1/4 plate
    kerf-.05
    feed- 45 ipm
    pierce delay-2 sec
    pierce height .188
    plunge-100 in/min
    cut height- .07
    pause at end of cut- 1sec
    Now go to options>select post processor> MP1000, and hit ok.
    It does the following.. goes to where we want to start the cut. the x and y works great. the Z how ever doesn't seem to work right. when it comes time to cut the the torch goes from being close to the table and goes up. making the numbers in mach become -(neg). seems to get near the top and homes out zero, then just brings the torch down to .188 from homing way up and then tries to start the plas.The only way we got it to cut was to bring the torch/plas from near the metal and watch the numbers. Then we changed the pierce height to aroun 17.3 and cut height to 17.0. It then cut.. what causes the -(neg) and homeing way up at the top???

    2. when it does cut a section it raises all the way up then moves then lowers, cuts, raises all the way up, moves then lowers.. It does thins on all the cut. what can fix that? I figured it should raise slightly from the table/metal move then go back down and cut again..


    3.the actual product we cut is a ring that goes around the outside bolt pattern on a chevy 1ton rear differential. so it should have been big.
    Problem was it cut it small enought to fit in the palm of my hand.
    WELL actually it only cut the inside and the bolt holes. It did not cut the outside ring..Sheetcam seemed to show the cut pattern of the outside and inside, but it didn't cut like that..
    questions;
    What causes the cut out to be small and not actuall size?
    How do I get more copies of the same product on to the sheetcam. I mean fill the 4x8 sheet with lets say 10 of the same cutouts..
    How do I make sure that sheet cam will cut both inside and outside?

    Tom I am going to go to your board in yahoo and maybe ask how does the torch height control work or how can we test it out? does the thc only work when it is actually running the plas and cutting?
    example we had 2 pieces of metal butted against each other and when the torch went from one sheet to the next it didn't raise up to compenstae for the height differenc of say a 1/16 to 1/4 diference..


    But we did get it to cut and and made the motors work a little faster...
    I am going to put a seperate post on here looking for any really knowledged folks in aout Spokane Wa area that know how to run both programs..

    And i seriously cannot thank you enough for your help.....

  9. #9
    Join Date
    Mar 2006
    Posts
    759
    In Sheetcam, when you load a job file or drawing, it asks if you want the file in inches or mm, check inches. Other than that, you must make sure you drew it to scale in your CAD program.

    I have made the mm to inch mistake in Sheetcam too many times to count, by accidently clicking on mm when clicking ok.(chair)

    I highly suggest reading the tutorials in the Help pulldown, but a quick writeup on nesting:
    after you have selected your layer, etc and have your path lines, etc for your part, go to the top right of your screen and click on the white Tee or cross shaped button. Now go down to your part and right click on it, and select duplicate. Place your duplicate wherever you want it, and keep doing that until your sheet is full. This is not a complete write up on it, but it should get you started.

    You can also select New Job instead of new drawing, make a few duplicates of that, and then open another New Job on the same sheet, say if you wanted 4 of the differential covers for the Chevy dually, and 4 for S10 differential covers, all on the same sheet.

    Make sure when you draw these parts that they are all on the same layer, that could be why the outside didn't cut, either that or you have an incomplete line path somewhere, for instance a straight line and a curve not joined up together properly.

    If nothing else, PM me, and email me with your drawing, and the Sheetcam file you wind up with. I will see what I can do for you
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    "If the women don't find you handsome, they should at least find you handy"
    -RedGreen show.

  10. #10
    Join Date
    Jul 2005
    Posts
    2415
    Quote Originally Posted by drink2mny View Post
    Massa and Torch.. Thank you guys for the input..
    Torch/Tom I think My buddy has been in contact with you. Blackbird ring a bell?


    Now go to options>select post processor> MP1000, and hit ok.
    It does the following.. goes to where we want to start the cut. the x and y works great. the Z how ever doesn't seem to work right. when it comes time to cut the the torch goes from being close to the table and goes up. making the numbers in mach become -(neg). seems to get near the top and homes out zero, then just brings the torch down to .188 from homing way up and then tries to start the plas.The only way we got it to cut was to bring the torch/plas from near the metal and watch the numbers. Then we changed the pierce height to aroun 17.3 and cut height to 17.0. It then cut.. what causes the -(neg) and homeing way up at the top???.....

    Where do you have the Home on Z? The MP1000 Post in SHeetCAM assumes you are using a touch-off (floating head and switch) and a HOme moves goes towards the material and finds the top then backs off the "switchoffset", Zero's the DRO (at this point the tip should be sitting on the top of the material or close to it.) It then raises to the pierce height (.188) fires the torch and then moves quickly to the Initial cut height (parameter in SheetCAM). At that point the MP1000 takes over control of the Z (well actually tells MACH how and where to move the Z because MACH never "releases" control of Z) Depending on the state of the toolpath MACH can (and does) ignore the commands from the MP1000.



    2. when it does cut a section it raises all the way up then moves then lowers, cuts, raises all the way up, moves then lowers.. It does thins on all the cut. what can fix that? I figured it should raise slightly from the table/metal move then go back down and cut again..
    Sounds like either the Z direction is reversed (numbers should ALWAYS be positive on the Z DRO in MACH) and moving up should make the numbers increase while moving down makes them decrease. Once again they should never go negative unless your material is warped enough that it one part is actually lower than where the torch started.


    3.the actual product we cut is a ring that goes around the outside bolt pattern on a chevy 1ton rear differential. so it should have been big.
    Problem was it cut it small enought to fit in the palm of my hand.
    WELL actually it only cut the inside and the bolt holes. It did not cut the outside ring..Sheetcam seemed to show the cut pattern of the outside and inside, but it didn't cut like that..
    questions;
    What causes the cut out to be small and not actuall size?
    How do I get more copies of the same product on to the sheetcam. I mean fill the 4x8 sheet with lets say 10 of the same cutouts..
    How do I make sure that sheet cam will cut both inside and outside?
    Put the objects that are to be an inside cut on one layer in SheetCAM and use the inside cut process for those objects. Cut them first in the process list. Make the outer cut another layer and setup a separate cut process for that layer and make it in outside cut.

    If the image is the right size (you can measure using the cursor and the numbers at the bottom to keep up with XY postion) then the cut will be the right size.

    Make sure you are not getting metric sizing mixed with inches. Make sure all packages are in the same system: MACH, SheetCAM and Drawing. Actually a DXF is just scaled in "units" and you have to tell it on import if it's inches or mm. SheetCAM will give you the option.

    Have you calibrated the table and you know an inch is exactly one inch in movement on all axis?

    Tom I am going to go to your board in yahoo and maybe ask how does the torch height control work or how can we test it out? does the thc only work when it is actually running the plas and cutting?
    example we had 2 pieces of metal butted against each other and when the torch went from one sheet to the next it didn't raise up to compenstae for the height differenc of say a 1/16 to 1/4 diference..
    We can answer the THC questions on our Support Site. I also end up answering "How to cut with a Machine Controlled Plasma" a lot and then there are the MACH and SheetCAM questions

    In order to raise up 90 degs instantly you would need to have a vertical rate of astounding speed. Think about it. The torch is moving along horizontally at 2 or 3 inches per second. Now, it doesn't have forward looking radar! It would have to sense the voltage change when it hit the "wall" and instantly pull the torch up a vertical cliff. Physics says it can't happen. Even a 45 deg incline cut would require the Z be able to move as fast as the X and Y are moving. You are asking the machine to do something that is impossible.

    Do not try to lay out material of different thicknesses or even separate pieces of material. The spaces between will drive the THC nuts and you already know what will happen when you try to make it climb a verticle wall.

    Plasmas are made for cutting contigious material that has waves and slopes of 30 deg or less. You could soup up a Z axis with a big old servo with say 800 IPM of vertical speed and cut material at 100 + IPM and climb a 45 to 60 deg angle, but not a 90!

  11. #11
    Join Date
    Mar 2006
    Posts
    759
    Tom, just curious, but couldn't you have two separate sheet thicknesses on the table, load all the job files, and have one job file set up with a different tool and therefore a different process in Sheetcam? Say,load one file at the bottom of the sheet in Sheetcam, and the second file at the top of the sheet, with a different setting for each, corresponding to the position of the plates on the table? I know this can be done in Sheetcam, can it be done with the THC?
    Say insert code that would allow for a manual jog onto the new (thicker/thinner) material before continuing to cut?
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    "If the women don't find you handsome, they should at least find you handy"
    -RedGreen show.

  12. #12
    Join Date
    Jul 2005
    Posts
    2415
    Quote Originally Posted by massajamesb View Post
    Tom, just curious, but couldn't you have two separate sheet thicknesses on the table, load all the job files, and have one job file set up with a different tool and therefore a different process in Sheetcam? Say,load one file at the bottom of the sheet in Sheetcam, and the second file at the top of the sheet, with a different setting for each, corresponding to the position of the plates on the table? I know this can be done in Sheetcam, can it be done with the THC?
    Say insert code that would allow for a manual jog onto the new (thicker/thinner) material before continuing to cut?
    As long as you treated the two pieces as separate jobs and raised the head before you went from one sheet to the other a touch off (floating head) would work fine. You just can't run along a piece of material at 100 IPM and expect the head to travel up and over and verticle wall.

    As fast as plasma cuts it would seem to me to be more productive to cut one size of material and clear the table and cut the other.

    The THC is only involved in keeping the torch at the correct height as it cuts. All of the positional moves in Z are handled in SheetCAM. The THC dosn't even cut in until about .5 second after a vlaid pierce and the start of a cut. Only changes in the THC to cut different thicknesses of material might be the tip volts (arc gap). All other parameters (things like feedrate and pierce height) are part of the CAM program.

    Tom Caudle
    www.CandCNC.com

Similar Threads

  1. Need Quick Answer!!
    By WilliamD in forum Laser Engraving / Cutting Machine General Topics
    Replies: 2
    Last Post: 10-17-2006, 05:39 PM
  2. Simple Question Simple Answer ?
    By p3t3rv in forum Stepper Motors / Drives
    Replies: 6
    Last Post: 02-16-2006, 04:00 PM
  3. If you can ... answer this please
    By cncbox in forum DIY CNC Router Table Machines
    Replies: 9
    Last Post: 08-12-2005, 02:50 PM
  4. easy to answer question
    By senor J. in forum Mach Software (ArtSoft software)
    Replies: 2
    Last Post: 01-28-2005, 01:34 AM
  5. ask for answer
    By lijiuhua in forum Community Club House
    Replies: 0
    Last Post: 01-05-2005, 02:29 AM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •