[pinguS]

Hi all

Just a curious question, luckily we are having a full 5 axis machine being brought in, with the Heidenhein blah blah control. For which I am going to get Solidcam to produce a post processor for.

Just wondering after reading a few web pages, I hear that most 4 and 5 axis programming is done with inverse time feed? Is this true. I sort of understand why, because when you move XYZ then normal feed will do, but soon as another axis is input, then maybe the control just zooms up the feed on the extra axis. i.e. if you were milling around a sphere lets say, and the actual tool movement is only about 0.5mm in XYZ, but about 190 deg in C, then without inverse, the machine will move 0.5 at feed programmed and just increase the C axis feed? Is this true, does solidcam calculate this correctly if inverse is needed?

Or when you use HSS,HSM and 5 axis module, should the post always use inverse just in case?

any info would be helpful

Also if anyone could, post a few lines of 5 axis G code, to see if I'm understanding this right.

pinguS

[jess fuqua]

yes you are correct inverse time feed is needed in order to keep your speeds and feeds the same when rotating your rotary table. I had my post made to only use inverse time feed during rotary movement only. On my Haas machine inverse time feed is G93 and inverse time feed off is G94. So my program during simultaneous 4th and 5th axis machining will switch back and forth between G93 and G94. Below is A little sample of some Simultaneous machining using inverse time feed.


N7694 X0.0874 Y6.7438 Z0.7837 A-87.562 B179.503 F1187.0492
N7696 X0.0881 Y6.749 Z0.7368 A-87.958 B177.131 F1195.5186
N7698 G94 Z0.7366 F24.
N7700 G93 Y6.6991 Z0.7346 F480.
N7702 X0.088 Y6.7015 Z0.6605 A-88.591 B177.184 F4564.7573
N7704 X0.0878 Y6.7033 Z0.5558 A-89.486 B177.16 F3097.927

[pinguS]

Ok, but would this be the situation on all controls, reason I ask is because on another machine we have a 4th axis unit simultaneous, but only really cut aluminium, so never really checked if the machine was going too fast or slow. On that I modified the FANUC post to give normal Gcode feed rate, should I revert back to inverse. Don't know what came over me!!!

Im assuming most if not all controls (fanux, siemans, etc) need inverse for 4/5 axis work.

I believe solidcam are going to visit to do machine site check, to measure etc when it has arrived, to create accurate post etc. I'm assuming they will create a post which does Inverse feed.

Another question, Solidcam, being computerised, obviously is clever enough to know that when the feed is input, it actually calculates on that regarldless of number of axis used, although CNC controls need inverse, being slightly "thick" maybe??

[jess fuqua]

Read this post, Machines & Machining engineering - Inverse time feed rate

[Brakeman Bob]

There is no need to use inverse time with the Heidenhain TNC 530. I have only used inverse time with older (pre 30i) Fanuc controls.

What machine are you getting and what is the H'hain control fitted? Also, do you plan to use CYCLE 19 for 3+2 operations or PLANE SPATIAL? This is an important issue as the PLANE commands are easier to deal with to my mind.

[jess fuqua]

Wow! The Heidenhain TNC 530 is one fancy control I've never seen one until today after watching a video on it.

[Brakeman Bob]

Once you get used to it, it's wonderful. I come from a Fanuc background and it took me a while to get my head around the logic that Heidenhain use as it seemed all arse backwards to me, but now I wouldn't go back to Fanuc for five axis programming for love or money. I've been programming in H'hain for nearly 6 years now and I am still discovering new things in the control, be it functions or new ways of doing things.
Enjoy!

[pinguS]

Hi

With regards to inverse time, I'm assuming the Heidenhein 530i control is clever enough to adjust feeds itself, without inverse time feed then? This is the control which will be on the machine, if Bob is right...

I have also noticed alot of people are moving away from Cycle 19 to Plane spacial, as I have never used Heidenhein, what exactly is this.

To get a heads up, can someone please post a very small program for the heidenhein, like, I dont know, 4 drill holes around a square block or something with few explanations, if anyone can be bothered !!

Also, I hear you can just clock the part on a heidenhein control and the machine will know how to rotate the part accordingly to the program, is this true, or does it need to be central on the table? (being a table/table machine) I cant understand how this would be possible, as solidcam would generate a program from the created MAC position, so machine should be set the same ?????

Lastly, I have also been told that the control has Software options 1 and 2, whatever this means I dont know, but I assuming Solidcam will create post to suit?

Long post I know...........

[pinguS]

Also found that the machine has a renishaw probing system, is this for inspecting the parts or for initial setup, I'm assuming that this has to be done outside solidcam, as like any other job?

[Brakeman Bob]

With regards to inverse time, I'm assuming the Heidenhein 530i control is clever enough to adjust feeds itself, without inverse time feed then? This is the control which will be on the machine, if Bob is right...

That's right, the control is clever

[/QUOTE]I have also noticed alot of people are moving away from Cycle 19 to Plane spacial, as I have never used Heidenhein, what exactly is this.[/QUOTE]

PLANE functions are a way of programming "3+2" moves that is very easy to write a post processor for as the machine resolves the 3 planar elements (as in Euler translational functions) into the A & C moves the machine needs to execute in order to achieve the desired orientation.

[/QUOTE]To get a heads up, can someone please post a very small program for the heidenhein, like, I dont know, 4 drill holes around a square block or something with few explanations, if anyone can be bothered !![/QUOTE]

See my PM

[/QUOTE]Also, I hear you can just clock the part on a heidenhein control and the machine will know how to rotate the part accordingly to the program, is this true, or does it need to be central on the table? (being a table/table machine) I cant understand how this would be possible, as solidcam would generate a program from the created MAC position, so machine should be set the same ?????[/QUOTE]

Absolutely true, the part does not need to be on the centre of the table and I have programs the first true up the C axis to get the part axes in line with the machine and then probe the part again to set the work zero. Imagine trying to do that in Fanuc.

Lastly, I have also been told that the control has Software options 1 and 2, whatever this means I dont know, but I assuming Solidcam will create post to suit?[/QUOTE]

Options 1 & 2 means that you have the optional functions such as graphics and DXF conversion available to you. I t shouldn't make any difference to your post unless you want it to.

What machine are you getting. I program for a Hermle (A & C axes) and Mikron (B & C axes) here, both with H'hain iTNC530 and I am willing to share what I can about 5 axis machining.

By the way, I consider a probe an essential piece of equipment on a 5X machine.

[pinguS]

Hi

Bob, we have looked at a few, Matsuura / Hardinge / DMG, etc. But by end of next week we will make the decision. All stock machines, so not problem on delivery, and more towards bottom end of market, i.e. 100 - 200kg table weights. I have specifically requested Heidenhein iTNC530 on the machines, boy does that jack up the prices. I have also looked at 2nd hand, but again as we're new to this, it may be preferable on new machine.
The kind of work we are going to be using is more that like max 4axis movement, but at least we will have the option of 5 if ever needed.

Does the probe do inspection work too on machines, and can this go into solidcam?

Also when you say clock the table, you use the probe to clock the table first, then you use the probe to clock the part. Then the control treats the part as being central. But do you not have to put the part in this position on solidcam?? so that it can check if the tool is going to hit the table when part off centre??

[pinguS]

Another question, do you tend to always use solidcam for heidenhain programming, or sometimes the conversational? Also how are you outputting from solidcam post, in g code or in heidenhain format?

[Brakeman Bob]

The probe can do inspection work while the part is on the machine but this cannot be programed in SolidCAM at this time (I understand that a probing module for SolidCAM will be available in the near future, but at what cost I cannot guess). I program our probing using Cimco EDIT, having built up a macro library of probing cycles. Where the fun starts is trying to output the results - read up the chapter on Q DEF's in the H'hain manual (btw, the H'hain programming manuals are available to download from their website FOC).

OK, 'clock the table'. With the part vaguely positioned on the table measure the angle of a face that should be parallel with the X axis (CYCL 420). Use the result from this to adjust the C Axis PRESET (don't use datums - more trouble than they are worth). Then run CYCL 247 and PLANE SPATIAL A0 B0 C0 TURN and the table will rotate to make the face previously probed parallel to X axis. Then probe your part to set zero where ever you want it to be - I recent programmed a part with X0 110mm from table centre.

As for SolidCAM, if you are using MachSim for collision checking or over-travel checking, then you need to position the part in SolidCAM at it's theoretical position on the table but for everything else, no, you can just have zero's in the MAC.

We use H'hain conversational, there is a lot more functionality available to you in my mind. But do not bother trying to use the contour functions - just let the post output a profile as a series of lines and arcs. Drill cycles in H'hain are a piece of cake, as is threadmilling.

[pinguS]

Yeah, just looked at the program output you sent, talk about totally different from G code, I think I will download the manual and see what each line is doing. Looks interesting, now its a matter of time, until we receive a machine.

So using the probe, you can have the part slightly off angle, probe it to straighten it. Then probe the part again to get your positions for the MAC positions or zero position. Then move the part the same amount on Solidcam, for error checking. Have I read this correctly?

So my understanding about the posts you have generated from Solidcam, you have it posting Conversational code? is this right. Also I'm assuming on the machine, even if the post is conversational, you can still dig in to look at g code, or are they just 2 different programming options all together.

If your posting in conversational, that would mean the post created by Solidcam, would more than likely have everything Heidenhain can do... so its fully transparent between the two?

[Brakeman Bob]

Not quite. I program my part in SolidCAM and also model the fixturing so I can do collision checking. Because my fixturing is modelled I can calculate the theoretical position of the work zero. When the part is loaded on the machine the actual positions may be 0.2 / 0.3 or ½° different to the theoretical positions - enough to scrap the part - so I probe the part to reset the work zero and then carry on machining.
The code I sent you is straight out of my post processor and is as conversational as is possible from CAM. There are other conversational features such as FK contours but I think these are more aimed at people programming at the machine. Let's be clear, there are 2 different manuals for H'hain conversational and ISO programming and the suffix of the program when saved is different. I suggest that you download the H'hain Programming Station software and have a play with the control - it only costs money if you want to program more than 100 lines of code. I would also suggest that you get some training in H'hain as I found it invaluable in understanding the logic behind how the control does things (which is in a very different way to Fanuc indeed).

I don't know quite what you mean by "fully transparent". My post pumps out conversational code and can do everything I want it to do except create calculations using Q DEF's (that I do manually in Cimco Edit). The big differences between ISO and conversational lie in drill cycles, tool calls and the ability to have incremental and absolute co-ordinates on the same line. The Polar co-ordinate system is also very useful betimes.

[pinguS]

Hi

When i say transparent, i meant that what processes heidenhain can do, solidcam virtually copies, which obviously is not the case, and is limited to the post being written how you want it. Either way, I'll download H'hain Programming Station and see how I get on.

I will ask the machine supplier regarding starting training.

Once you have realigned your part on the table, do you re input the alighned offsets back into Solidcam, or do you just realign and carry on machining, within reason obviously, i.e. if the part is super complex then I can understand re inputting into solidcam.

[Brakeman Bob]

Once you have realigned your part on the table, do you re input the alighned offsets back into Solidcam, or do you just realign and carry on machining, within reason obviously, i.e. if the part is super complex then I can understand re inputting into solidcam.

No, I don't the actual values into SolidCAM as they are usually small - certainly less than 0.5mm and you only need the theoretical values for collision checking. I'm not brave enough to take the spindle closer than 2mm to 'fixed' items, the discrepancy is irrelevent.

In H'hain 5 axis programming, both 3+2 and simultaneous, I find it best to have just one work zero (or PRESET in h'hain speak) and in SolidCAM this is MAC 1 POS 1. I then define a different POS position about MAC 1 POS 1 for each of the 3 + 2 orientations and these are posted out as PLANE SPATIAL commands. For 5X sim, you use MAC 1 POS 1 for everything.

[pinguS]

I just downloaded the H'hain Programming Station to give it a try, my first thoughts.....................


aaaaahhhhhhhhhhhhh WTF

[Brakeman Bob]

Make sure that you enable the on-screen keyboard and study the key map in the manual. I didn't when I first got it and I had exactly the same reaction as you.

I found it really useful once I got going as it forces you into the correct syntax.

[pinguS]

I have enabled the onscreen keyboard, what next, its like looking at something so random. I've gone into the help files, but where to start. I am looking at booking onto h'hain programming course in london, once we get machine. But as a simple starter, I know this is irrelevant to Solidcam, but I have downloaded the programming station, got keyboard up. Can anyone give me a simple step by step on there to, lets say drill a hole at position X50. Y39. or something like that....