PDA

View Full Version : first time mach3 post issue?



williamsmotower
12-05-2011, 06:02 PM
here is start of a post I made in madcam using mache inch post processor.

I used 0,0,0 for machine position before posting, and have my machine set at all 0's.

look at this gcode madcam gave me.... isn't z axis going to try and move + 7".269" before starting?

G00 G49 G40.1 G17 G80 G50 G90 G64
G20
(.25 Flat end Center cutting 4 flute HSS)
M6 T1
M03 S0
G01Z0.000
G00X1.076Y0.487
Z7.269
G01Z7.144 F
Y0.517Z7.138 F
X1.051Y0.543Z7.132
X1.006Z7.124
X0.980Y0.517Z7.118
Y0.473Z7.110
X1.006Y0.447Z7.104
X1.051Z7.096
X1.076Y0.473Z7.089
Y0.517Z7.082
X1.051Y0.543
X1.006
X0.980Y0.517
Y0.473
X1.006Y0.447
X1.051
X1.076Y0.473
Y0.517
X1.051Y0.543
X1.006
X0.980Y0.517
Y0.473
X1.006Y0.447
X1.051
X1.076Y0.473
Y0.517
X1.078Y0.525
X1.083Y0.531
X1.091Y0.536

svenakela
12-06-2011, 04:32 AM
Have a look in one of the existing three M3-processors, make a post and see how they behave.
Why are you making a new one?

williamsmotower
12-06-2011, 11:00 AM
I used the existing Mach3 inch in madcam

Dan B
12-06-2011, 12:18 PM
Is your part 0 at world 0 in Rhino?

williamsmotower
12-06-2011, 01:07 PM
yes, part is zeroed in rhino... at bottom of part

Dan B
12-06-2011, 01:15 PM
If you would be willing to e-mail me your file, and your post, I could take a look. My address is cncdanb@gmail.com.

Dan

hub
12-06-2011, 01:25 PM
yes, part is zeroed in rhino... at bottom of part

Try zero at top of the part?

williamsmotower
12-06-2011, 01:55 PM
i emailed you the part and post Dan.

One thing I just noticed, i see that rhino isnt saving my settings for madcam. is there a trick to this... so everytime i open rhino it's already set-up?

Dan B
12-06-2011, 02:35 PM
Can you check what you sent me. I got the code, not the post, and the file didn't have any madCAM paths in it. It was just a simple cylinder.

Thanks,

Dan

Dan B
12-06-2011, 02:51 PM
Sorry, I missed your question.

I always set up the options in 2 places. First, in the Rhino options, then with the options command in Rhino. It always sticks for me.

I'll attach a couple of screen shots.

Dan

williamsmotower
12-06-2011, 07:06 PM
I sent you a new email Dan, thanks again

Dan B
12-07-2011, 06:05 AM
Can you take a screen shot of your post-processor window? I want to see if you are setting your home position Z value to 0. I suspect that your are. This is causing the tool to travel to 0 (which will smash into your material) then is traveling in the Z up to your very high safe clearance height.

G00 G49 G40.1 G17 G80 G50 G90 G64
G20
(.75 Flat end Center cutting 4 flute Carbide)
M6 T1
M03 S2000
G01Z0.000 <<<< this can be forced by changing the z home value
G00X-0.685Y-0.470
Z2.800 <<<< traveling back up to your super high safe clearance value
G01Z0.800 F60
X-0.683Y-0.457Z0.798 F60
X-0.686Y-0.427Z0.794
X-0.695Y-0.398Z0.790
X-0.710Y-0.372Z0.785
X-0.730Y-0.349Z0.781
X-0.754Y-0.330Z0.777

Take a look at that, and see if I'm on the right track. By default, madCAM should give you a value above the stock, so you might be shooting yourself in the foot if you are changing this. Of course, without seeing the post (not the code), I could be wrong. There may be issues with how the post is configured.

Dan

williamsmotower
12-07-2011, 09:46 AM
Did you get last email? Is this from that?

I'll screen capture it later, but I'm definitely changing xyz positions to all zeros on that post processor page.

Dan B
12-07-2011, 12:09 PM
Yes, I looked at the file with the madCAM paths. Try posting without changing those values and see if it makes more sense. I posted for one of my machines (without changing the home position) and it looked good.

Dan

williamsmotower
12-08-2011, 03:49 AM
it's same thing. Just not right... the z values aren't making sense.

Anyone know when Joakim will be back?

svenakela
12-08-2011, 04:57 AM
Try another processor and check if there's a difference. Use the iso for example.
I have never experienced this, I will try it out tonight when I'm back at my office space.

Dan B
12-08-2011, 05:51 AM
So you left the home values as they were, and you still got that Z0 move in the beginning? You are going to have to share that post of yours to narrow this one down. By post, I mean the post-processor file that you used to generate the code.

Dan

williamsmotower
12-08-2011, 10:30 AM
Mach 3 inch , also Mach 3 5axis inch does same thing.

I tried a fanuc, that made xyz look believable to me.

Dan B
12-08-2011, 02:22 PM
I posted the code with the mach 3 inch post, and I got good results. Take a look at the attachment, there may be something there that will help you see what's going wrong.

Let me know if this helps.

Dan

svenakela
12-08-2011, 05:25 PM
Did a test with the Mach3 post and it went fine too.

williamsmotower
12-08-2011, 07:54 PM
I won't be able to try it for about 2 hours . Do you hit enter after xyz inputs on post page?

williamsmotower
12-09-2011, 02:12 AM
Look at the X and Y in beginning of Gcode. I don't know why Z has changed now to a reasonable number... I did hit tab key after inputting dimensions. maybe madcam wasn't recognizing them before?

http://img.photobucket.com/albums/v250/williamsmotowerx/post2.jpg

now look at this page... are they related? My X and Y even though at 0 on post processing page start out at a high number in actual gcode... which would not work.

http://img.photobucket.com/albums/v250/williamsmotowerx/post3.jpg

svenakela
12-09-2011, 03:17 AM
There's nothing wrong here. Your model is placed at Origo in the workspace and X & Y movements in the post are correct according to your stock model.
I think you think that the "home" position in the post processing dialog is something else than what it really is. If you want to cut the model with Origo (0,0,0) somewhere else you have to move the model in Rhino to the wanted position, then post process.

williamsmotower
12-09-2011, 09:52 AM
How do you do that? Click cplane icon on madcam toolbar?

svenakela
12-09-2011, 10:32 AM
How do you do that? Click cplane icon on madcam toolbar?

The machine space is the same as the model space. You have Origo right in the middle of your model. Just select everything and move it where you want to have it when you're milling!
Check this:
MADCAMCNC: Moving around in space (http://madcamcnc.blogspot.com/2011/01/moving-around-in-space.html)

williamsmotower
12-09-2011, 02:32 PM
I was able to talk to turmite, the usa madcam re-seller.

we found my drawing wasn't set in a "world" position. I won't be able to play with this until later tonight... but if anyone has any tips to expand on this it may help many users out.

Rodent
12-09-2011, 07:06 PM
here's how I have my seed models constructed

http://i714.photobucket.com/albums/ww146/RegenerateGuitarWorks/Tools/CNC_WorkingSetupForBodies_Annotated.jpg

my first step was to map out my CNC XY working envelope, and then place that with the upper left corner at 'Home' (X0, Y0)

since I utilize locating pins as part of my design process, and since these are placed into my table, I have these included in my seed model. I also include the neck centerline and a perpendicular line placed at the scale length location. I place a point at this intersection location. all of the is at a Z=0 depth, since there is where I will set my Z-depth - all cuts on a side reference this for their depth.

for reference, I also have a standard body blank located in the up and flipped position.


when it comes time to cut a part I first send the spindle home and zero out the X and Y. I then manually joggle the spindle over the body blank I'm cutting and lower the Z until the cutter just makes contact with the wood. this is where I will zero out the Z depth

I'm now ready to go to work :)


there is no requirement to do it this way, but I find that for me it's the most sure way to always design a part that fits my table and is consistently located in relation to it's opposite side so that all machining operations are precisely aligned

YMMV of course

all the best,

R

Rodent
12-09-2011, 07:16 PM
I was able to talk to turmite, the usa madcam re-seller.

there are other MadCAM re-sellers besides this one, and each has their specific strengths and non-strengths.

your CAD/CAM/CNC experience level should be a considerable factor when choosing the re-seller you purchase from to ensure your level of support needs are included within the total cost picture. if you have little CAD/CAM/CNC experience, finding a re-seller with generous post-sale support may be more in-line with your actual needs than what is offered by a different re-seller with a bargain price but very little free post-sale deployment consulting

it would be a shame to self-sabotoge your MadCAM experience by ignorantly choosing to 'save' $50 - $100 on the initial purchase price. I'm not implying anybody has done this ... just providing topics for consideration for others who are researching their CAD/CAM/CNC deployment

all the best,

R

Dan B
12-10-2011, 05:32 AM
I was able to talk to turmite, the usa madcam re-seller.

we found my drawing wasn't set in a "world" position. I won't be able to play with this until later tonight... but if anyone has any tips to expand on this it may help many users out.

Yes, your Cplane is set to the center of the pin, but if you use the command Cplane World Top, you will see that the actual world 0 is shifted slightly. I apologize for not mentioning that earlier, but it is so instinctive for me to set that immediately that I do it without thinking. If you don't have an alias set up for that, you should.

I noticed that you set the home position to X0 Y0 Z3. Looking at the mach 3 inch post, I see that the X and Y are not "hooked up". Only changing the Z value will have any impact on the code.

As far as Rodent's comments on support, I'm not sure how to take that. All I can say for sure is that for madCAM support, you can always come here like you did. Support can come in various forms (reseller, developer, or users on a forum). Not everyone offering help does it for profit, or based off of where or how you purchased the software. Personally, I help because I want to see people succeed with madCAM because of the time and effort that I know has gone into developing it to this point. Also, the more satisfied users there are, the more word of mouth advertising will happen, which in turn may increase sales, which will result in more revenue to develop madCAM further, which is good for all of us.

Dan

williamsmotower
12-10-2011, 10:57 AM
that's how I feel Dan.. I want Madcam to succeed and grow. We're on the the ground floor of this project! (well I just put one foot in the door, lol) but the better this program get's we'll be able to reap the rewards.

I'm still having a hard time wrapping my head around this.

I have a 3 axis metal working mill. I want to machine a a 1" block in a 2" piece of aluminum held in a vise.

It sounds like I have to move vise into a position that is relative to my Rhino drawing. That to me is backwards. I should be able to have vise anywhere on table... move my axis to part... zero machine and run program.

Isn't this the normal way machining is done. Seems madcam is set-up for fixtured tables only. Why is Madcam set-up this way?

williamsmotower
12-10-2011, 11:03 AM
Dan, what do you mean my XY are not "hooked up"

Dan B
12-10-2011, 01:59 PM
It sounds like I have to move vise into a position that is relative to my Rhino drawing. That to me is backwards. I should be able to have vise anywhere on table... move my axis to part... zero machine and run program.

Isn't this the normal way machining is done. Seems madcam is set-up for fixtured tables only. Why is Madcam set-up this way?

madCAM works just like other CAM programs. Create your model with your datum at world zero and you can put your vise anywhere. Just pick up the corresponding point on your material, call that your machine zero, and away you go.

On our Trak LPM, we have 2 vises, and we definitely don't need to move them to match Rhino. We routinely machine large fixture bases on our Awea 3016, and we don't use vises at all. We clamp right to the table. madCAM is the only software we use for programming that machine. We also program our Haas, couple Fadals and 6 Hermles with madCAM (although we do use WorkNC primarily for the Hermles).

What I meant by not hooked up is that the variables in the post that use the X and Y home position values are not there. There are a lot of variables, and not every post uses them all. In this case there isn't an "xhome" or a "yhome" variable in place, but there is a "zhome".

Dan

svenakela
12-10-2011, 04:17 PM
Lets put it this way, there are many ways of doing the same thing. There are no static procedure to come to the end result - a complete milled mould for example. The example I linked to earlier in this thread when the model is moved in space is just one way of doing it. We actually run most of our machines as a fixed table and I rarely work with world zero in the middle of the part. Did that with your last two CAM programs as well.
madCAM is naughty powerful, the future enhancements are way above most of the users and their machines capability. There are some basic features I wish comes in later on, but how many in this forum (cnczone as a whole) have a workshop with 4 or 5 axis machines? i know a bunch of madCAM clients that have it, they do some really heavy things with this software.

Now back to the problem. :)
I'm not sure anymore. What is the problem?..

svenakela
12-10-2011, 04:29 PM
... on our Awea 3016, ....

You have a 3016?! You make me pretty jealous.

Dan B
12-10-2011, 04:45 PM
You have a 3016?! You make me pretty jealous.

How about 5 Hermles, with #6 coming this Wednesday? Does that make it worse? :-)

williamsmotower
12-10-2011, 04:56 PM
there is a problem. the z starts at zero... then moves up 1.142"

why does it move to 1.142"?

it is just cutting air. it will not cut the part

G01Z0.000
G00X-0.229Y0.541
Z1.142
G01Z1.017 F60
X-0.185Y0.525Z1.010 F60
Y0.568Z1.003
X-0.449Z0.961
X-0.625
Y0.525
X-0.581Y0.541
X-0.537Y0.553
X-0.518Y0.558
X-0.493Y0.562
X-0.449Y0.567
X-0.361Y0.567
X-0.317Y0.562
X-0.293Y0.558
X-0.273Y0.553
X-0.229Y0.541
X-0.185Y0.525
Y0.568
X-0.449
X-0.457Y0.566
X-0.463Y0.561
X-0.468Y0.553
X-0.472Y0.543
X-0.475Y0.531
X-0.477Y0.518
X-0.477Y0.504
X-0.477Y0.491
X-0.475Y0.478
X-0.472Y0.466
X-0.468Y0.456
X-0.463Y0.448
X-0.457Y0.443
X-0.449Y0.442
X-0.405Y0.445
X-0.361Y0.442
X-0.317Y0.435
X-0.282Y0.427
X-0.273Y0.424
X-0.229Y0.408
X-0.182Y0.384
X-0.140Y0.357
X-0.119Y0.340
X-0.096Y0.320
X-0.074Y0.297
X-0.052Y0.270
X-0.045Y0.297
Y0.688
X-0.052Y0.693
X-0.758
X-0.765Y0.688
Y0.297
X-0.758Y0.270
X-0.735Y0.297
X-0.714Y0.320
X-0.691Y0.340
X-0.669Y0.357
X-0.625Y0.385
X-0.581Y0.408
X-0.537Y0.424
X-0.529Y0.427
X-0.493Y0.435
X-0.449Y0.442
G00Z1.149
G00X-0.737Y-0.294
Z1.142
G01Z1.017 F60
X-0.759Y-0.268Z1.012 F60
X-0.765Z1.011
Y-0.355Z0.997
X-0.758Y-0.360Z0.996
X-0.669Z0.982
Y-0.356Z0.981
X-0.714Y-0.320Z0.972
X-0.723Y-0.311Z0.970
X-0.759Y-0.268Z0.961
X-0.765
Y-0.355
X-0.758Y-0.360
X-0.669
Y-0.356
X-0.714Y-0.320
X-0.723Y-0.311
X-0.759Y-0.268
X-0.765
Y-0.355
X-0.758Y-0.360
X-0.669
Y-0.356
X-0.714Y-0.320
X-0.723Y-0.311
X-0.759Y-0.268
G00Z1.149
G00X-0.114Y-0.335
Z1.142
G01Z1.017 F60

svenakela
12-10-2011, 05:42 PM
Then i think Dan is on the right track.

This is taken directly from the help file (Post processing->Post process):
Home position: The cutter position for start and return. ( Variables must also be set in the postprocessor, else it has no affect )

Further down in the chapter Post processing->Creating and Editing:
"xhome" // Home position set from postprocessor dialog.
"yhome"
"zhome"

"_xhome" // Home position without output character.
"_yhome"
"_zhome"


In the Mach3_Inch post processor there are no references to any home variable in the early stages. There's only a reference to zhome in the tool change procedure.
What you could do is to add following to your file as the first steps in the *FIRST_CUT* section
G00 "zhome"
G00 "xhome""yhome"

Try that and see if it works.

EDIT: You actually should put the changes in a *FIRST_MOVE* block.
*FIRST_MOVE*
Place lines for the first move after tool change or before next toolpath.
*END_SECTION*

williamsmotower
12-10-2011, 06:52 PM
like this?

"x""y""z"
*END_SECTION*
*TOOL_CHANGE*
("toolname")
M6 T"toolnr"
M03 S"speed"
G01"zhome"
*FIRST_MOVE*
"xhome"
"yhome"
"zhome"
*END_SECTION*
*TOOL_STOP*
M5 M9
*END_SECTION*
*PROGRAM_START*
G00 G49 G40.1 G17 G80 G50 G90 G64
G20
*END_SECTION*
*PROGRAM_END*
M30
*END_SECTION*
*LINE_START_NUMBER*

svenakela
12-10-2011, 06:57 PM
Nooo... I didn't write that.

*FIRST_MOVE*
G00 "zhome"
G00 "xhome""yhome"
*END_SECTION*

Change to this and try it out. I'm leaving for the bed now (1 am).

williamsmotower
12-10-2011, 07:02 PM
still not working. i tried it in a few places... still have z going up (this has been edited to your last post #39)

G00 G49 G40.1 G17 G80 G50 G90 G64
G20
(.25 Flat faced Center cutting 4 flute HSS)
M6 T1
M03 S2000
G01Z0.000
G00 Z0.000
G00 X0.000Y0.000
G01X-0.229Y0.541Z1.017 F60
X-0.185Y0.525Z1.010 F60
Y0.568Z1.003
X-0.449Z0.961
X-0.625
Y0.525
X-0.581Y0.541

williamsmotower
12-10-2011, 10:36 PM
ok, got it.

mach3 post seems to be working fine... it was the world issue. I copied part, put it in a new drawing, and re-did everything. something was screwey in the rhino file.

just cut my first part. everything went smooth so far.

thanks for all the help!

svenakela
12-11-2011, 04:22 AM
Ok, I thought you'd tried that already! :)

Dan B
12-11-2011, 05:01 PM
Glad to hear you got it working.

Dan