Straight line tool paths for limited memory controller

nikoneer · May 14, 2020

We have an old mill with a Heidenhain Tnc 145 controller for simple jobs. Most of our work can be done with conversational programming, but we are looking at a simple CAM software for the slightly more complicated parts. Since the memory of the 145 is very limited, is there any software that can be forced to generate straight line movements as much as possible instead of the optimized curves that are most efficient? I'm aware that tool life and productivity will suffer, but that's okay.

Skickat från min ELE-L29 via Tapatalk

Mike1974 · May 14, 2020

With Mastercam you can turn on filtering and adjust to your hearts desire, although it will still probably generate some arcs, unless you are literally milling straight lines... but then you don't need cam?

I am a little confused by your question.

1) Mastercam is not really simple (or cheap)

2) Set up a drip feed (DNC) if possible so memory isn't an issue

3) I would *think* most cam systems have some way to filter code to optimize(?)

nikoneer · May 14, 2020

The 145 can't do drip feed, otherwise that would be the way to go...

I've tinkered a bit with SolidWorks CAM and HSMXpress, but I couldn't make any of them do what I want. Might be I haven't found the method yet.

Think of a part where I want to remove quite a lot of material. If doing it by hand it would be a number of simple straight cuts of different length and depth, followed by a more complicated finishing. The CAM systems all seem to optimize by machining in arcs with constant step over, which can make a 4 G-code line straight cut into 400 code lines of small segments...

Skickat från min ELE-L29 via Tapatalk

gustafson · May 14, 2020

First, mention the name of the control you seek help with in the title, you will get higher quality answers

I know fusion can be made to create small enough programs to run in the controls 1000 line limit.

It will also output conversational, which is much more compact than other forms

The size of the program will be mostly up to you and how you create toolpaths

Do NOT use straight lines, or it will be huge

Do not try to use helical ramps

Do not use multiple passes, the software creates a new separate output for every pass

The 145 cannot to 3 axis simultaneous moves, so true profiling is not happening, but within the 2 1/2 axis world you can do much if you watch how you create the toolpaths

ONECNC also does conversational output

13engines · May 14, 2020

1) Turn off line numbers. Not needed and wastes memory.

2) Segmented arcs programming is way more memory intense then arc moves. Use arcs and force them to use R instead of I and J unless that gives you trouble. R derived arcs uses fewer characters per move.

3) Use as large a tool as possible for each part feature including the heaviest step over and depth of cut you can manage.

4) Try to create continuous tool paths with fewer retracts and resets to Z height.

5) If possible, force the software to not repeat Modal Commands. G0 - G1 - G2 - G3 - F - X -Y -and Z for instance are Modal on many controls. Don't repeat them when not necessary.

6) Create and use Subroutines when working multiple parts and/or fixture Offsets.

Every little bit helps.

Dave

Mtndew · May 14, 2020

Can you use Macro programs?

Mud · May 14, 2020

I'm looking at Smartcam for exactly that reason. The underlying tech dates back to the old school smartcam of years ago, which gives great control over the toolpath geometry, instead of creating tons of sculpted moves that you can't control. Plus you can draw a simple line for a toolpath and generate code from it instead of drawing the edge of the part and referring to it and just accepting what the program produces.

If you do look at Smartcam, I'm interested in hearing back what you find. I used it extensively years ago, haven't tested the new version yet.

nikoneer · May 14, 2020

Mtndew said:
Can you use Macro programs?

I certainly can't, maybe I have some colleague that can. How can we use that wisely?

Skickat från min ELE-L29 via Tapatalk

nikoneer · May 14, 2020

By the way, there are very few postprocessors for the 145 around, as far as I have found. HSMXpress has one that seems okay, but the problem is still my lack of control over the tool paths... Of course one can be created or modified to work, but that's an investment among many others

Skickat från min ELE-L29 via Tapatalk

Mud · May 14, 2020

One here for Smartcam for a Kondia and another for a Wells Index w/145 - Smartcam MIlling Code Generators

And yes that's an issue these days for any but the latest controllers.

gustafson · May 14, 2020

You can usually use a post for a 151 or 155 with a 145

BUT the 145 is super fussy

It actually needs all the characters in the correct location
In a 151 if you skip numbers it jsut condenses the program. IOW if you use a line editor to remove ten lines of program so the file looks like:

1 L X
2 L X
12 L X

In the 151 it will go back into the control as:

1 L X
2 L X
3 L X

In the 145 you will have 10 blank lines
1 L X
2 L X
3
4
5
6
7
8
9
10
11
12 L X

it also IIRC wants character locations to be just so.

neilho · May 15, 2020

I run a 151A, FWIW.

Another possibility is VisualMill, which has a postprocessor for Heidenhain conversational that works for the 151. Maybe it'd work for your 145.

Programming by hand makes for the simplest code.

Search

Largest Manufacturing Technology Community on the Web

Search

Straight line tool paths for limited memory controller

nikoneer

Plastic

Mike1974

Diamond

nikoneer

Plastic

gustafson

Diamond

13engines

Stainless

Mtndew

Diamond

Mud

Diamond

nikoneer

Plastic

nikoneer

Plastic

Mud

Diamond

gustafson

Diamond

neilho

Titanium

Similar threads