Anilam conversational post FIX

[HughesTooling]

Edit 03/03/2015 updated attachment see latest post for changes.

I've fixed a lot of errors in the Anilam post.
List of changes.
IJK needed to be output as XCenter, YCenter and ZCenter.
Added helical moves all planes.
Added spiral work around to reduce code size.

Work offset 0 recalls the machine home, change so only 1 to 9 are output. If 0 offset is used in the setup in HSM no offset is output so whatever offset the machine is set to wiil be used.

No modal output for planes or moves. Added 2 new functions "writePlaneBlock()" & "writeMoveBlock()" to replace G-code with the correct Anilam words.

Fixed drill cycles. XY coordinate are not on the same line as cycle set up, moved to next line. No dwell in drill cycles changed to use boring cycle. Fixed chip breaking and deep drilling to correct format.
Set start and return to same height and ZDepth to cycle.bottom

Added quillDRO to properties if you have 3 axis and a coupled DRO on quill set to true and program will pause so you can retract quill before move to Z home.

Changed M code output so it outputs "Mcode"

Commented out RPM output as it's set in the tool table on the machine. When I have time I'll put a setting in properties to make easier changes.

Changes in post are commented with "HT" and date.

I've tested what I can, if you spot any problems let me know.

Mark

[matthew.nichols]

This is some good stuff Mark!  Thank you for sharing!

[AchimN]

Thanks for sharing this. That means there are a lot of issues in the generic Anilam post? If yes, we will update the generic post of course.

[HughesTooling]

Yes there was quite a lot wrong.

I have a question about helical moves, I have a file to use as a test and some helical move are linearized and some come out as helical and I can't see what's different. The moves at line 332 "1001.m" and 582 "1001.dmp" linearize but line 354 "1001.m" and 598 "1001.dmp are helical. I've set the post to use all 3 planes for helical moves so are moves the linearize not on 1 of the planes and how can you tell in the dmp file.

This helical move comes out as helical


These moves linearize


Mark

[HughesTooling]

Test file attached. G code above is from posting Contour1 only. Post that outputs comments attached as well.

Mark

[HughesTooling]

I've added in a couple more things.

In properties I've added 3 options.
1. outCool set to true M codes to turn coolant on off will be output

2. outRPM set to true spindle speed will be output

3, quillDRO set true program will pause to retract quill before rapid to home.

Mark.

[fishtruk]

Thanks Mark, I tried out your post. I changed the easy stuff. Changed the extension to .cnc which my 1100 looks for.

I also remmed out the lines setting the Mcode since the Anilam doesn't need them.

Odd thing is the spindle starts about 5 lines after the Tool# 1 is read.

What Anilam do you have and is this an issue?

Thanks Again!
Nelson

[Laurens-3DTechDraw]

fishtruk wrote:
Thanks Mark, I tried out your post. I changed the easy stuff. Changed the extension to .cnc which my 1100 looks for. I also remmed out the lines setting the Mcode since the Anilam doesn't need them. Odd thing is the spindle starts about 5 lines after the Tool# 1 is read. What Anilam do you have and is this an issue? Thanks Again! Nelson

I think it would be an easy test on your machine if it is an issue.

[HughesTooling]

I have a 3300m and on my machine the tool call starts the spindle. At the start of the program I get something like this.

* 1001
* GENERATED BY FUSION 360 CAM 2.0.1484
* WEDNESDAY, MAY 13, 2015 091836
* TOOL 4  D=6 CR=0 - ZMIN=-1.962 - FLAT END MILL
* TOOL 5  D=3 CR=1.5 - ZMIN=-3.5 - BALL END MILL
* TOOL 9  D=3 CR=0 - ZMIN=-3 - FLAT END MILL
* TOOL 18  D=1 CR=0 - ZMIN=-2.212 - FLAT END MILL
Dim Abs
Plane XY
Unit MM
Tool# 0
Dwell 0.0
* RETRACT QUILL
Rapid  Z0
* 2D CONTOUR4
Tool# 4
Mcode8
X0.03 Y-28.191 Z15.003
Z5.003
Line  Z1.003 Feed 200.

In the tool library on the machine I have tool 4 set to FWD so as soon as it's called it starts. What are you seeing in the code that starts the spindle.

Mark.

[fishtruk]

Thanks Mark,

There's some really strange stuff happening at the machine. It stops, says feedrate zero on a line number But there is no federate change on that line !!

The code is so bloated that I have to run DNC and can't edit it on the machine. The machine doesn't want Tool #'s except perhaps for direction and offsets. It works fine if I put in an Mcode 8 and Mcode3

I'm trying to make the moves non modal. Perhaps to fix a problem. I want Line or Rapid at the beginning of every block where appropriate.

[HughesTooling]

If you change the writeMoveBlock function to this it will give modal moves.

function writeMoveBlock() {
 var words = formatWords(arguments), rwords, planeword;
     if (words) {
		 switch (arguments[0]) {
      case "G0":
			planeword = /G0/g;
			rwords = words.replace(planeword, "Rapid ");
			writeWords(rwords);
	   break;
      case "G1":
			planeword = /G1/g;
			rwords = words.replace(planeword, "Line ");
			writeWords(rwords);
	   break;
      case "G2":
			planeword = /G2/g;
			rwords = words.replace(planeword, "Arc Cw ");
			writeWords(rwords);
	   break;
      case "G3":
			planeword = /G3/g;
			rwords = words.replace(planeword, "Arc Ccw ");
			writeWords(rwords);
	   break;
	   default:
			writeWords(arguments);
	 }
//	writeComment(arguments[0])
	gMotionModal.reset();
    }

}

I've added

	gMotionModal.reset();

to the end of the function.
Also for testing it might be easier to use a 2d contour so you can edit at the machine.

Mark

[HughesTooling]

I've modified a post to give non modal output and spindle control. At the top of properties there's an option A1100 set it to true and see if that works.


Mark.

Edit. Updated post attachment needed to add M5 code at tool change.

[fishtruk]

Thanks a lot Mark,

That seems to work fine.

I have found why it would stop and read Feedrate=Zero. The Internal Accuracy in the setup was too large.

I still don't know why it stops now and then and gives Error-Radius Too Small for Given Endpoint...The Guy at Heidenhain doesn't seem to know why either. When I put the numbers in CAD, Start point, End point and Radius, it works out Exactly. I've fooled with the Arc correction amount in the setup but to no avail.

Nelson

[HughesTooling]

I have the offline programing software for the 3300m and I had a program the other day that ran fine in the offline software but the machine gave an error, both had the same settings for accuracy and arc correction! Although the machine gave an error warning it ran ok so I didn't investigate to much. The arc that gave me the warning was for a vertical lead in, any idea if the problems you've seen are in the XY plane or in one of the vertical planes.

Mark.

[fishtruk]

It was XY.

I don't get warnings, it just stops. I wish I got warnings.

The fellow I mentioned suggested I run it until it stops, then increase the radius by .001 and try again.....Fine except this program is a bloated 4000 lines of code...could take forever. Nice if I could pick up where it left off, but in that case I'd have to stay by the machine and get it going when it stops...

[HughesTooling]

Hi Nelson

Can you get the file on the machine using the serial connection and run a simulation. Also is the 1100 based on a PC like the 3300m. I've fitted a IDE to compactflash reader to get big files onto the machine. There is a bit of a compatability problem that means you have to copy the files from the compactflash disk to the hard drive though.

Here's a link to the drive I'm using.
http://www.addonics.com/products/aeudmacf.php

Mark.

[fishtruk]

Can you get the file on the machine using the serial connection and run a simulation. No...machine has a 1 meg 16 bit ISA card for the long term mem. I have to use DNC for anything over about 200kB.

Also is the 1100 based on a PC like the 3300m. I'm sure it is. but it has a 386-25 cpu

I've fitted a IDE to compactflash reader to get big files onto the machine. There is a bit of a compatability problem that means you have to copy the files from the compactflash disk to the hard drive though.I've been talking to Jerry Bouvain from Heidenain about upgrading this machine to a 486-66 and adding a CF to the IDE bus instead of the ISA mem card. I think it would act just like the ISA card in that I think I could just upload a file into the CF and run it. I have 16 Meg of ram in this machine...1 Meg of "disk" and 16 Meg of ram....go figure...

[fishtruk]

Hey Mark,

I have the strangest problem. My 1100m just stops at certain arcs. Not all but when it stops the Radius is 0.05

I've sent a file to the expert but he has no idea. If you wish see if this program errors out with a "bad" radius. Line 919 is the first one...change the radius to 0.051 then run again, it will stop at line 970...Cad says the numbers are perfect. Setup numbers aren't the issue.

It's been posted with your latest, but that isn't the issue. I get this with a Bobcad post from Bobcad.

I have to be out of touch until next week.

Thanks either way! Your IV post is the best yet.

Nelson

[HughesTooling]

Hi Nelson

Tried your program and got the same error. Have you tried posting with useRadius set to no so you get circle centres instead.

Also what CAM are you using if you're using Fusion can you upload a file.

Mark

[HughesTooling]

Ok I've figured out the problem, I modified the post so spiral moves are converted to arcs if they are within a tolerance. It all works fine if you use circle centers instead of R. I'd recommend you use circle centres if you can because I've done a lot of work to reduce code size using that method.

If you want to keep using R edit the post and set allowSpiralMoves to false, but the program size will increase!

When I get some time I'll change the post so use R stops the spiral conversion so you can use either way.
Mark.