NC File Numeric Precision

[saabaero]

Just wondering if anyone has experienced something similar to what I have...

I am using the latest Tormach postprocessor for creasting NC files with Sprutcam Version 7. When I look at the NC files that are created the coordinates for the axes consist of numbers with 3 decimal places in spite of my having my Sprutcam system tolerance set to 8 decimal places.

The strange part is that for circular inperpolation using G2 and G3 commands the "I" and "J" parameters consist of 5 decimal places but the X,Y&Z coordinates are 3 place decimals. At first I thought that my axes values just typically consisted of only 3 decimal place as they normally do in my designs (except for fractional values - I usually specify them as 4 place decimals - i.e. 0.3125"). The other thing I noticed was that adjusting the cutter diameter in the tool selection in Sprutcam by 0.0001" or 0.0002" still resulted in 3 place decimal values for the axis coordinates.

Is this a function of the Tormach postprocessor or something I am doing wrong? I would expect that I should be able to get 4 decimal place accuracy for small parts with the PCNC mill.

[Cairns]

Adding something possibly related to the question: Every time I open one of my projects in SprutCAM it displays some very poorly worded pop up dialog with a question about changing the precision of my drawing from 3 decimal points to 4 (and now 5 points in the newest version). It's unclear whether clicking Yes changes the project I'm opening to a higher precision or lower but no matter which way I answer the question, I always get prompted again the next time I open it. Any thoughts on how to make this go away and hopefully default all my projects to 4 decimal points? I've already set my preferences to reflect 4 points of precision.

Saabaero, is it possible that you are getting this question as well and it is changing your default setting?

[saabaero]

Yes it is possible since I get the same message whenever I open a previously saved project regardless of the precision set in the settings when it was saved. You are correct about the question in the dialog box being ambiguous but I think it is asking to change a file saved in a lower precision to the current higher precision.The question is how do you set what precision the file is saved as? You would think it would be the same as the setting it was created in.

Regardless, I still see the coordinates in the NC file as 3 decimal places with a new file I created with an 8 decimal place setting. A key that the precision is correct in the project file is when I use the measure command. The precision of the measured values and coordinates are shown in the precision I chose in the project settings.

[Cairns]

I did some work last night and can confirm that I'm seeing the same results as you.

[RTP_Burnsville]

Same issue here and also with that annoying popup dialog box talking about precision (3 vs 5 for me). I have the all-post version and briefly looked at the Tormach driver and noticed a tolerence variable had a value of 3. I tried to change it to 5 but could not save it. I have not had time to investigate fruther.

Where I noticed an issue is when calculating the feed rate. If one gets the chip rate too low the calculated feed value is set to F0 by the post process. This appears to be a rounding issue with the 3 tolerence digits and puts an F0 into the Gcode. Needless to say if that happens (and you don't catch it)everything just hangs and one gets to restart.

If I remember right there is another post here from several months back about the pop menu and possibly this same issue.

Robert

[saabaero]

Thanks for the replies! At least I'm not the only one seeing this issue.

I did forward my initial post to Tormach for them to comment on.

I agree, F0's are not a good thing to have in a NC file. They really extends the machining time considerably!

[mayhugh1]

Hi all,
There are three places in the Sprutcam workflow that determine the precision of the coordinates output in the G-code. The first is in the Measurement units tab of the Setup menu of Sprutcam. I use Imperical units exclusively and I have the indicated precision set to 5 (places to the right of the decimal.) The second place can be tricky. It is in the machine parameters for the particular machine you are using. Under Control Parameters ->Tolerance(digits) you will find a number here which by default in Sprutcam is 3 digits (to the right of the decimal). This defaults to 3 digits because it is a reasonable number for metric units which is what Sprutcam assumes by default. You can change this to 5 units as if you are an Imperical units user as I am. You must change it before you bring in your model and start defining macine operations, though. Choosinig your machine and setting this parameter should be the very first thing you do after launching the application. This default value of 3 is contained in the machine xml file (one file for all machines) and if you change it there you won't have to remember to change it each time you start Sprutcam. There is a tutotial on the Tormach site about how to customize Sprutcam's xml files. The third place that affects the outputted precision is in the postprocessor. Sprutcam's postprocessors allow a total of 8 digits maximum to be used to hold a coordinate register's output, i.e. x,y,z. Because the Tormach postprocessor was designed to handle metric/Imperical units transparently, a value of 4 digits to both the right and left of the decimal was selected by default. You can certainly modify this if you are using the all posts version but I wouln't recommend this unless you you kow what you are doing. Writing Sprutcam posts isn't for the faint-hearted. So, if you're only seeing 3 digits to the right of the decimal of your G-code, you are probably not setting the machine parameters to 4 or more digits. If you are setting this parameter, then you are somehow using a very old version of the Tormach postprocessor. A change to 4 digits to the right of the decimal from 3 digits was made some three-four years ago.

I agree about the very confusing message box that you sometimes see. Usually this message is warning you that you are trying to open a project with the current machine precision parameter set to a different value than were used to create the project you are trying to re-open. For me this was typically an "aw-sh*t" message which usually meant that I had forgotten to properly set the machine precision when I originally saved the project and now I have to start over. After I learned about the machine xml trick, I haven't seen this message again.
If you are a mixed metric/Imperical user you will see a similar message when opening a metric project with the current units set to Imperical or vice-versa. It is asking if you want to convert the units. Unfortunately if you allow it to try to convert the units, not everything gets converted and you can run into some pretty confusing things later in the workflow, especially in the lathe operations. It is best to stop and change the current units to match those of the project.

With respect to the feedrate, only 4 digits total are used in Sprutcam's postprocessors to output the Feedrate or F value. The Tormach post uses all four digits to the left of the decimal and so feedrate values less than 1 are rounded down to 0. I modified the version I use to 3 digits to the left and 1 digit to the right so I can output feedrates less than 1. I submitted the modified post to Tormach a few years ago but they weren't hearing complaints from other users and probably felt there was less risk leaving things as they are. Another problem that I seem to be the only one having is that the current post spins my fourth axis in a direction opposite to the direction that it should. I made many successful 4th axis parts until one day I tried to cut a complicated assymetrical part and discovered the issue. I modified the post I use to correct this also, but have not heard of a single complaint from another user. - Terry

[Cairns]

With regards to seeing only 3 digits of precision in the GCode.

Go to the Machining tab
Tormach
parameters
machines tab
Tormach
Control Parameters
Tolerance (Digits) is set to 3

I changed it to 4 and now see 4 points in my Gcode.

[bevinp]

Hi Terry,
You may be inerested in a problem I had today that I found to be related to the tolerance setting.
The code produced by SC 7 for a pocketing operation would not load into to Mach3 because of a zero radius occurred in G3 command. After producing the code again (with the same result), and scratching my head (and various other parts of my body), I wondered if it was the tolerance difference between SC and Mach3. And yes it was. After I changed the tolerance from the SC default 3 digits to 5, Mach 3 loaded the new code without complaint.

I guess it was a rare event that the G3 maths reduced to zero radius because of the tolerance. But I am very pleased that this forum is so active with valuable information.

Thanks very much for your wisdom.

Regards,
Bevin