Denford AutoCAM

Matt · Post by **Matt** » Thu 17 Aug , 2006 13:52 pm

Hello

I am trying to install Denford AutoCAM v1.10.

The programme installs fine but it won't install the triac Pnc3 post processor.

I run the Mpost.bat file and select triac but it just comes up "No file name given" or "file not found". There is a file called Pptriac.exe but I can't to do anything with it.

Is there anything I can do?

Could AutoCAM be added to the download list?

Mr Magoo · Post by **Mr Magoo** » Fri 18 Aug , 2006 22:33 pm

AutoCAM must be getting on for 20 years old now and by todays standards is a VERY basic CAM package. it will trace a profile and drill holes and that's about it. No cutter comp, no area clearance cycles so I wonder if it's worth the effort of trying to get it running

Denford have other low end CAM packages that are far superior - just make sure they output through their Universal Post Processor and they'll be able to generate progs for your Triac

Or contact -=PAB=- on this forum - I know he's doing similar things.

Matt · Post by **Matt** » Tue 22 Aug , 2006 9:41 am

I know what you are saying about being basic but it will do all I need at the moment. The version I have does have radius compensation and circular and rectangular area clearance.

I just want to import dxf files and control where the tool will start to cut etc. I have MillCAM but is has no radius comp or anything.

I was all set to purchase QuickCAM 2D but I will have to create my own postprocessor. Is this hard? But QuickCAM doesn't seem to let me create open tool paths with radius comp!

Post by **Denford Admin** » Tue 22 Aug , 2006 14:17 pm

QuickCAM doesn't seem to let me create open tool paths with radius comp

Because of the way the toolpath offseting works - it needs to create closed areas which can be used to determine whether the object is an island of another object or not. Its been designed to make life easier - you just select all your shapes, and the program will decide whether to fill the shape internally or externally automatically.
See example:

Simply select all the shapes in area clearance and it knows which ones to fill - very useful for text shapes

If this is a problem, you can trim the resulting area using the boolean tool, or by the secret trim command (CTRL-T)

I will have to create my own postprocessor. Is this hard?

No - its easy enough - just have a look in:
C:\Documents and Settings\All Users\Application Data\Denford\Posts
There is a text file to help explain the settings in the *.ppl files
- just looking at the current files (in Notepad) will make it much clearer as to how the post is configured.
Just copy one that gives the nearest output, rename it and play with the settings until you get what you want - just remember that all QuickCAM will send out is:
XY arcs (G02 G03) / feed moves (G01) / rapid moves (G00) / spindle request (S4000) / tool request (T0101) and all these codes and number formats can be changed by the post config file

Mr Magoo · Post by **Mr Magoo** » Tue 22 Aug , 2006 22:36 pm

Hi Matt...

I've just installed AutoCAM v1.10 (I'd forgotten just how primative it is!!!)

I tried this...

Run MCAM.BAT
F1 -> Load MILLDEM.DXF
F1 -> Load Profiles
F1 ->Create CNC

These steps created a MILLDEM.MGP file in your MCAM folder - it's the intermediate file the Post Processor will translate into your machine-specific CNC file.

Run MPOST.BAT
Select TRIAC

This translated the MILLDEM.MGP into a MILLDEM.TRI file.

BUT HERE IS ANOTHER PROBLEM!!!
The AutoCAM post processor has created a Binary file that can only be sent to your Triac machine using the OLD TRIAC offline programming software (you cant use Ind Text Editor or the Triac software that's on Denfords webiste)

It's all turning into a bit of a nightmare!!!

I really don't think this is going to work....

Matt · Post by **Matt** » Wed 23 Aug , 2006 14:09 pm

Hello Mr Magoo

Thank you for time humouring me. I think I will have to accept defeat on this one!

I will probably go with the QuickCAM in the end. It does look very good but it still troubles me that you can not do open paths with comp. This something I use a lot to rebate edges of parts, or to begin cutting off the job and lead in. I sometimes need to control where the cutting starts and ends.

I have tried creating my own post processors, but its the arcs and circles that confuse me. The software just seems to do it so differently to my machine eg IJK?

Anyway....Many thanks

Triac whizz · Post by **Triac whizz** » Wed 23 Aug , 2006 17:58 pm

Try this

http://www.dolphin.zenwebhosting.com/products.htm

good value does & what it says on the box

and there's a post processor for Triac

and good support

No connection - just a satisfied customer

Post by **Denford Admin** » Thu 24 Aug , 2006 9:07 am

Triac Whizz is probably right - the Dolphin stuff looks more industrial - it depends what you're making.

QuickCAM is aimed for use by school kids and the main purpose of the software is to let them make things as quickly / easily / painlessly as possible, ie, they don't care about lead-ins / outs, they just want to make a plastic sign for their bedroom door with their name on it.
Its still very capable - especially if you want to do circuit boards or already have DXFs, but lacks features you may want, say, if you were cutting steel.

If you post a typical program that works on your machine, I should be able to make a post file for it .

Matt · Post by **Matt** » Thu 24 Aug , 2006 10:28 am

The Dolphin stuff does look very good, but I was really just looking for something "flexible" rather then "sophisticated".

I think I will go with QuickCAM and take you up on the offer to help with the post.

I can always work around the inflexibly if I need to by editing the code manually afterwards. I had thought it would be very good for PCBs.

Matt · Post by **Matt** » Thu 24 Aug , 2006 13:43 pm

I just purchased QuickCAM.

I would be very grateful if you could produce a post processor for me (and others).

This code was created in MillCam and works fine on my machine. It is a square, circle and arc. It has the file extension .pnc

I am using the Industrial Text Editor to transfer to the machine. This requires an "L" to be added at the end of each line. Is this something that could be included in the post?

G90

G71

M6T1

M3S1500

G0X10Y50

G0Z2

G1Z-1FZ100

G1Y10FX150

G1X50

G1Y50

G1X10

G0Z2

G0X110Y30

G1Z-1

G3X90Y50CX90Y30

G3X70Y30CX90Y30

G3X90Y10CX90Y30

G3X110Y30CX90Y30

G0Z2

G0X120Y10

G1Z-1

G3X150.355Y45CX115Y45

G3X150Y50CX115Y45

G0Z2

M5

G0Z100

M2

Post by **Denford Admin** » Thu 24 Aug , 2006 16:21 pm

Hi,

Have nearly got it - but I'm going to have to update the application to allow for absolute circle centres (looks like that facility was never thought about):

Check if this (straight out of QuickCAM) would work .... (NB, the centre points are incremental in this example still)

Code: Select all

G90L
G71L
M5L
M6T0101L
M3S23000L
G0X50.000Y10.000L
G0Z2.000L
L
G1Z-2.000FX1250L
G2X79.606Y90.369CX-1.842Y46.316F5000L
G1X80.000Y90.000L
G0Z2.000L
G0X76.750Y94.235L
L
G1Z-2.000FX1250L
G3X76.750Y94.235CX33.250Y45.765F5000L
G0Z2.000L
G0X40.123Y70.000L
L
G1Z-2.000FX1250L
G1X180.123FX5000L
Y200.000L
X40.123L
Y70.000L
G0Z2.000L
G0Z2.000L
M5L
M2L

Also, I'm not sure if the trailing 000s and blank lines (L) are a problem ?

(added:-)
- this should be a bit closer now:

Code: Select all

G90L
G71L
M5L
M6T1L
M3S4000L
G0X50.000Y10.000L
G0Z2.000L
G1Z-2.000FX63L
G2X79.606Y90.369CX48.158Y56.316L
G1X80.000Y90.000L
G0Z2.000L
G0X76.750Y94.235L
G1Z-2.000FX63L
G3X76.750Y94.235CX110.000Y140.000L
G0Z2.000L
G0X40.123Y70.000L
G1Z-2.000FX63L
G1X180.123FX250L
G1Y200.000L
G1X40.123L
G1Y70.000L
G0Z2.000L
G0Z2.000L
M5L
M2L

Matt · Post by **Matt** » Thu 24 Aug , 2006 17:04 pm

Hi there

Looks promising!

No it didn't like the (L) on the blank lines.

It seemed ok with the trailing 000s.

It errors 21 (circular move not within a quadrant) at the G2.

It doesn't like the lines near the end without a Gcode command.

When you say update the application do you mean QuickCAM itself?

Matt · Post by **Matt** » Thu 24 Aug , 2006 17:06 pm

Just seen added after posting!

Will check it out.

Post by **Denford Admin** » Thu 24 Aug , 2006 17:12 pm

When you say update the application do you mean QuickCAM itself?

Yep - most things can be changed in the post file by the user, but as there isn't a facility to change the circle centre type

, then the Post code embedded into QuickCAM will have to change as well.

- the next version with a few tweaks is about to be released, so it'd be great to get these changes in as well.

Matt · Post by **Matt** » Thu 24 Aug , 2006 17:19 pm

The second code works fine apart from the circles.

It will be great if you can include the change in the update so I can use the software. Any idea when it might be?

Mr Magoo · Post by **Mr Magoo** » Thu 24 Aug , 2006 21:41 pm

Just thought I'd add my two penneth worth...

1) Triac only accepts arcs within a single quadrant.
So a Clockwise arc going from 11o'clock to 2'oclock must be split into 2 NC blocks...

first from 11o'clock to 12o'clock
Second from 12o'clock to 2o'clock

So obviously a CW arc from 11o'clock to 7o'clock must be 4 x NC Blocks

2) It's a 2 1/2 axis machine so Z axis feedrates must be defined seperatly to the XY feedrates. I think that your block that reads
G1Z-2.000FX63L
may be moving the Z axis at the last defined Z axis feedrate, not at 63mm/min

A single Z axis move should be like this
G1Z-2.000FZ63L

And a 3 axis linear move should be like this...
G1 X10 Y20 FX80 Z-2 FZ63 L
X&Y axes move along a vector at 80mm/min whilst Z moves independantly at 63mm/min

I say linear move because you can't guarantee the Z axis will arrive at the end point at the same time as the XY axes. I guess you should do something like...

Not allow the post to output 3 axis linear moves and report an error or write a comment instead
calculate the XY feedrate and Z feedrate independantly based on the length of the vectors (it will almost output a true vector )

Mr Magoo · Post by **Mr Magoo** » Thu 24 Aug , 2006 22:27 pm

Or another option could be to write a QuickCAM post that generated an intermediate file for the old Universal Post Processor

And use the UPP to support the legacy machines - it already does all the segmented arcs and vector feedrate stuff.

Let me know if you want to go down this route - I can probably knock something up for you

Post by **Denford Admin** » Thu 24 Aug , 2006 22:27 pm

Argghh - old machines

3 Axis linears -
Shouldn't be too bad as QuickCAM only outputs XY or Z moves anyway - theres no need for 3 axis interp. I presume you can go rapid all 3 at once (not interpolated ?) ,eg, G0 X10 Y20 Z30

The other two issues will be easy enough to implement as options in the post.

ETA for the new version is sometime next week

Mr Magoo · Post by **Mr Magoo** » Thu 24 Aug , 2006 22:34 pm

3 axis G00 moves are fine

Post by **Denford Admin** » Tue 29 Aug , 2006 16:07 pm

Hi, This has just come straight from current BETA QuickCAM 2D - give it a try and let me know (max Z cut is 2mm - billet 250mmby250mm)
I could send you some pre-release files which will get your machine working if you want ?

Code: Select all

G90L
G71L
M5L
M6T1L
M3S4000L
G0X75.271Y24.161L
G0Z2.000L
G1Z-2.000FZ63L
G2X50.678Y61.484CX91.296Y61.484FX250L
G2X91.296Y102.102CX91.296Y61.484L
G2X131.914Y61.484CX91.296Y61.484L
G2X123.909Y37.272CX91.296Y61.484L
G0Z2.000L
G0X167.473Y54.190L
G1Z-2.000FZ63L
G2X156.613Y81.427CX196.199Y81.427FX250L
G2X196.199Y121.013CX196.199Y81.427L
G2X235.784Y81.427CX196.199Y81.427L
G2X196.199Y41.841CX196.199Y81.427L
G2X177.295Y46.646CX196.199Y81.427L
G1X175.932Y47.423L
G0Z2.000L
G0X140.404Y97.330L
G1Z-2.000FZ63L
G1X138.754Y98.981FX250L
G3X95.264Y116.524CX95.264Y53.845L
G3X38.897Y81.258CX95.264Y53.845L
G0Z2.000L
G0X24.780Y128.257L
G1Z-2.000FZ63L
G3X30.000Y127.639CX30.000Y150.000FX250L
G3X52.361Y150.000CX30.000Y150.000L
G3X30.000Y172.361CX30.000Y150.000L
G3X7.639Y150.000CX30.000Y150.000L
G3X24.780Y128.257CX30.000Y150.000L
G0Z2.000L
G0X28.066Y187.792L
G1Z-2.000FZ63L
G3X30.000Y187.639CX30.000Y200.000FX250L
G3X42.361Y200.000CX30.000Y200.000L
G3X30.000Y212.361CX30.000Y200.000L
G3X17.639Y200.000CX30.000Y200.000L
G3X28.066Y187.792CX30.000Y200.000L
G0Z2.000L
G0X10.000Y220.000L
G1Z-2.000FZ63L
G2X30.000Y240.000CX30.000Y220.000FX250L
G2X50.000Y220.000CX30.000Y220.000L
G0Z2.000L
G0X100.000Y220.000L
G1Z-2.000FZ63L
G3X80.000Y200.000CX100.000Y200.000FX250L
G3X100.000Y180.000CX100.000Y200.000L
G0Z2.000L
G0X110.000L
G1Z-2.000FZ63L
G3X130.000Y200.000CX110.000Y200.000FX250L
G3X110.000Y220.000CX110.000Y200.000L
G0Z2.000L
G0X130.000L
G1Z-2.000FZ63L
G3X150.000Y200.000CX150.000Y220.000FX250L
G3X170.000Y220.000CX150.000Y220.000L
G0Z2.000L
G0X141.250Y165.848L
G1Z-2.000FZ63L
G2X147.608Y153.385CX132.215Y153.385FX250L
G2X147.594Y152.736CX132.215Y153.385L
G0Z2.000L
G0X131.945Y154.428L
G1Z-2.000FZ63L
G3X115.873Y167.962CX115.327Y151.003FX250L
G0Z2.000L
G0X106.992Y166.693L
G1Z-2.000FZ63L
G3X96.839Y145.480CX124.075Y145.480FX250L
G3X100.647Y131.589CX124.075Y145.480L
G0Z2.000L
G0X85.844Y154.005L
G1Z-2.000FZ63L
G2X84.787Y158.234CX93.775Y158.234FX250L
G2X88.382Y165.425CX93.775Y158.234L
G0Z2.000L
G0X169.165Y150.621L
G1Z-2.000FZ63L
G2X188.220Y168.128CX188.220Y149.004FX250L
G2X207.345Y149.004CX188.220Y149.004L
G2X189.604Y129.930CX188.220Y149.004L
G1X189.043Y129.897L
G0Z2.000L
G0Z2.000L
M5L
M2L

Denford Software & Machines

Denford Software & Machines

Denford AutoCAM

Denford AutoCAM