1. Home
  2. ⋐⋒⋐ Computer Numeric Control
  3. Run your probe from your cam!

Run your probe from your cam!

********start********

var#20 = .2500 (input the diameter to probe); var#21 = 1.2500 (input x center); var#22 = 1.2500 (input y center); T20 (gets probe); P1001 (probe X size sub, result in var#1); P1002 (probe Y size sub, result in var#2); if var#1 > 3.5003 M00 (checks for X size); if var#2 > 2.0003 M00 (checks for Y size);

**********end*******

Put this somewhere you can easily cut and paste it, or make a simple macro, or customize a hotkey, whatever your cam system does to automate, otherwise just cut and paste it. Every cam system will allow you to add comments to the NC code.... find where the window to the cnc code is, hopefully in some kind of operations manager. Now your ready to rock.

Program up your part. Cut and paste the code into the window that puts comments in your cnc code at the end of an operation. Edit the first three lines for the hole you want to pick up, hit accept!

Stick this anywhere at will. Program your probe from your cam with ease!

****

AND dont EVER use an indicator to put something on location so it can be used to calibrate the probe like a ring gage. If you do that...think about it...

Reply to
vinny
Loading thread data ...

yep. The newer the probe the more easy it is. Its all getting standardized/

Reply to
vinny

I started running a 5 axis mill recentlly. We soon found out QC did not have the programing skills or a CMM big enough to quickly inspect the larger parts coming off the new machine. My CAM system (Esprit Mold) has a CMM feature that lets me output XYZIJK (point and vector) data be picking points on the model. I tried to get QC to figure out how to use the points to program the CMM to speed up inspection but they never did. We looked at buying a protable CMM arm (ROMER) but QC desided they would not have anything to do with it.

One day I was looking on Renishaws site and read about the InspectionPlus ($1076)macros. I found a PDF that talked about the XYZ single surface probing macro (9821) where you position the probe along a vetor normal to the surface of the point you need to measure. I already had a probe that could do 3D probing (MP700) all I need to do was find a way to take the XYZIJK data from EspritMold and use it to create a program using the macros to inspect the part.

With me brothers help I made this

formatting link
it takes the XYZIJK data and creates a program to inspect my parts in the machine. Here is a video of the machine cutting and probing the surface.

Best viewed with VLCMedia Player.

formatting link

Reply to
Mc Woodhouse

Probe programming can be crazy fun. Collecting the data is only the first step. The next step is using the data to manipulate work offsets by figuring out angles or locations. I have modified more than one mastercam post to output all my macro calls via the custom drill cycles.....yet I still have to custom write the logic to adjust whatever I am trying to do. As far as it being standardized....look at the difference between a Fanuc/Siemems/Heidenhan /Tosnuc, ect. To say they are similar is a broad generality. No way will one macro run on the other without massive amounts of editing. The logic may be similar...as in 1+1=2, but the calls to do so are very different.

Reply to
Zymrgy

I started running a 5 axis mill recentlly. We soon found out QC did not have the programing skills or a CMM big enough to quickly inspect the larger parts coming off the new machine. My CAM system (Esprit Mold) has a CMM feature that lets me output XYZIJK (point and vector) data be picking points on the model. I tried to get QC to figure out how to use the points to program the CMM to speed up inspection but they never did. We looked at buying a protable CMM arm (ROMER) but QC desided they would not have anything to do with it.

One day I was looking on Renishaws site and read about the InspectionPlus ($1076)macros. I found a PDF that talked about the XYZ single surface probing macro (9821) where you position the probe along a vetor normal to the surface of the point you need to measure. I already had a probe that could do 3D probing (MP700) all I need to do was find a way to take the XYZIJK data from EspritMold and use it to create a program using the macros to inspect the part.

With me brothers help I made this

formatting link
it takes the XYZIJK data and creates a program to inspect my parts in the machine. Here is a video of the machine cutting and probing the surface.

Best viewed with VLCMedia Player.

formatting link

****** So I could click on a point on my 3d cad model, and get a readout of it. xyzijk. Punch that into your proggy and a 3axis mill with a 3d renishaw will probe it and get a zero? hmmmm.... We have a few mills with that 3d probe on it that do pre-heat treat milling. How cool would it be to include an inspection program of 5-10 spots with my cnc program.

What's the popen command from, what controller are you on?

And where do the results of the probe go?

neat man. A+ work.

Reply to
vinny

POPEN stands for PRINT OPEN this creates a file to write the measurement results to PCLOS closes the file. I have Fanuc 31i control. I set the DATA I/O parameter so it outputs to the memory card. I just pull the card out of the control and view the report on my PC. Every line that has a W1 gets written to the card. Some of the code at the beginning and end is specific to my control but every thing from POPEN to PCLOS would be exactly the same as any other mill that has the Renishaw InspectionPlus macros.

You need to make sure the IJK is a "vector of 1" from the model origin. The IJK is a point in space (XYZ) that is 1 (in or MM) from the model origin not the point you are probing. So I0,J0,K1 would be straight down in Z or a point at X0 Y0 Z1, Hope that makes since.

Reply to
Mc Woodhouse

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.