These two settings are in sprut 7 as well, what they are for is a mystery here too.......
I have not seen this before and maybe it came with a recent update version.
SC10 tool library has a pre-assigned value listed for each tool; Length Corrector & Radius Corrector that seems to correspond with the tool number for an unknown reason.
The SC10 manual does not mention this, nor does it show it as such.
Any idea what these values mean?
-uman
Similar Threads:
These two settings are in sprut 7 as well, what they are for is a mystery here too.......
mike sr
I have looked at those over the years as well. The only thing that I can think of is that they are a form of "wear correction" or off nominal correction for the tooling that you are using. I never change the values there and only specify the measured diameter if it is more than 0.001" off. Quite frankly measuring wear loss/deviation of a ball end mill's radius would be a PITA :-). If one is trying to hit high tolerances for a 3D surface while machining moulds, however, having the ability/flexibility to program for it and compensate the G-code generated is probably a welcome feature.
They are the fields for setting where the NC program calls the tool length & tool radius compensation from
Normally they are the same as the Tool #
The length corrector appears in the NC program as a H#, and is associated with a G43 command ie G43 H1 Z1. will add the value stored in Length Offset #1 on the next Z move
The Radius corrector appears as a D# in certain operations only ie contouring when you need minor adjustment to achieve size because the tool may be smaller than programmed
- it is activated with a G41 / G42 code ( ie G41 D1 X--- Y---) usually only on a line move, & is de-activated with a G40 code ...... read the machine control manuals for more info
- radius comp should not be used when pocketing etc
- compensation only applied on the active plane ie G17 (XY), the other axis is a depth position
- it is not a 3D compensation- doesn't work on a ball nose radius, only the tool's diameter
These may / may not apply to you, but if you see them in your programs, it could open other options if needed
In my very limited experience, I set up the tool in the table in the machine software for tool length, the diameters are set in my cam, when I regrind a cutter, or want a bit of diamerer correction I change that in diameter window for that tool in cam or in the stock setting window for that particular op
This may not be the correct way but it works for me.
mike sr
I am trying to comprehend what Superman writes and what I am reading here. I need to get comfortable with this, so I am running tests on a simple program with different correction numbers and compensation options and reviewing the NC code.
MIke sr you are correct, this field was in prior versions of SC, only in a slight different location and field name. SC10 changed the name (compensation to corrector) and integrated this field with the Tooling 1 field and now I see it as important.
It appears this corrector number is only in play when compensation is ON (other than computer) so G41/42 start compensation and G40 cancel compensation are present in code.
What do the corrector numbers represent in value or effect?
When a new tool is added the corrector number is automatically assigned and matches the N-number. But this number can be edited. What happens then?
I spoke to Tormach SprutCAM tech support and he gave me this;
The Length Corrector assigns Correction (tool) number offset value to the selected tool <interesting as Superman stated>
The Radius Corrector has no effect in any Tormach post as of this date
Apparently, If tool #1 has correction value of 2, then tool #1 will assume tool #2 offset value; this could be catastrophic.
They recommend the following:
All tool numbers are to match the Corrector number for length and radius
Always select Computer compensation
I looked at my root library and found several tools with correction faults.
I ran some test code and could not affect the radius or length of the tools by altering the length or radius correction values, but PathPilot may think different.
-uman
Uman,
Good idea to keep a close eye on the tool length corrector number!!!!!
I have found sprut will assign some goofy number that IS NOT THE TOOL NUMBER. This is another error that the user needs to watch for that can cause problems and has imho no real application to the average tormach mill user. I have a large note book that details many of these and other settings that either generate NO code or cause errors in code and have no real world use for a tormach machine I recommend this for long term use of this program.
I have been working in the 4th axis section for couple months now figuring out what works and what settings generate code and witch ones do nothing. The amount of information on this area is thin and requires the user to figure it out step by step or take some advanced sprutcam class if there is one.
The SC library phenomenon is probably attributed to a user action - direct or indirect. I visit the root library often to observe those indirect effects and learn why.
Yea MH. CAM creativity requires complex control and SC certainly has that, unfortunately SC manipulation of those controls is often ambiguous мой друг. I am determined to achieve a master level of CAM control with SC. F360 is an awesome CAD/CAM, but like you, I use Alibre Design for the past 10yrs and F360 is dissimilar. I if figure the time investment to master F360 CAD/CAM is greater than the time to master SC - I hope.
-uman
Correct but,
it depends on your machine, yes a lot of machines have same H and D values and have special tables (right next to the tool height you would have a comp D value), but many Fanuc controls do not have a different H or D, thus require a D always different then the H, a lot of machines just have a offset table and you could use them for D or H, which means the machine can not tell difference between them its just data.
These values become important based on machine and post used, so for me its very important and all my tools that would use any compensation have different values, and normally I have offset the D's following after the tool change number so if you have 30 tools, the D's start from 31 and continue on, so tool 1 = H1 D31 for example.
I agree,
The earlier controllers don't have the H / D fields.....they are the GEOMETRY and WEAR offsets
....the #1 WEAR offset is ADDED to the #1 GEOMETRY offset to give a total offset for that offset number.....this is why the H[offset number] MUST differ form the D[offset number]
( I do use a D number that is 30 higher....but you could use one that is 2 pages later - so that your cursor stays in the same field )
--- BUT you will find it best if the T# ALWAYS MATCHES the tool length (H0 offset number.
( create your own procedure.....and rigidly stick to it......& apply notes in your program, if you (on occasion) have to alter numbers from your standard.