peter ~

Turning off retract between operations?

Recommended Posts

Hi guys,

When we are running our programs at our work, there is a return to machine Z home between operations, the spindle goes up to the max Z with an #MCS Z0, next it feeds down to the part using the tools plunge rate. If we did not detect any settings that would explain this behavior in the params or machine/control def , then is there a possibility we could fix this with post language? We need to fix this issue quickly it's costing us a lot of wasted CNC time If anyone has any Ideas what action I  should take I would so so appreciate it!!!

Thanks in advance!!

:alien:

Share this post


Link to post
Share on other sites
5 hours ago, peter ~ said:

Hi guys,

When we are running our programs at our work, there is a return to machine Z home between operations, the spindle goes up to the max Z with an #MCS Z0, next it feeds down to the part using the tools plunge rate. If we did not detect any settings that would explain this behavior in the params or machine/control def , then is there a possibility we could fix this with post language? We need to fix this issue quickly it's costing us a lot of wasted CNC time If anyone has any Ideas what action I  should take I would so so appreciate it!!!

Thanks in advance!!

:alien:

Yes, this is likely a Post issue. Typically the Post is setup to retract to Toolchange height, change the tool, then move to the XY start point (in rapid), the approach the Clearance or Retract Plane height, while enabling TLO (G43 Hxx Zzz). So the approach from Toolchange to start point should be in Rapid, unless you have "convert rapid to max feed" enabled.

Share this post


Link to post
Share on other sites
13 hours ago, Colin Gilchrist said:

Yes, this is likely a Post issue. Typically the Post is setup to retract to Toolchange height, change the tool, then move to the XY start point (in rapid), the approach the Clearance or Retract Plane height, while enabling TLO (G43 Hxx Zzz). So the approach from Toolchange to start point should be in Rapid, unless you have "convert rapid to max feed" enabled.

Hi Colin,

Thanks for the support, I checked the convert rapid to maximum feedrate is not enabled. Could you explain the TLO (G43 Hxx Zxx) or point me to a file or docs that would be relevant? I am not familiar with post language. Thanks!!

Share this post


Link to post
Share on other sites

What particular machine is this for?

TLO stands for Tool Length Offset.

In general, with a Fanuc-Style Machine, the following G-Codes are used to control positioning:

  • G00, G01, G02, G03 - Motion (Rapid, Linear, CW Arc, CCW Arc)
  • G17, G19, G18 - Planes (XY, ZX, YZ)
  • G40 / G41 / G43 - Cutter Compensation (XY Contouring Control) Programmed with a "D Value", which corresponds to the "Diameter Offset" being read for the XY adjustment.)
  • G43 / G44 / G49 - Tool Length (-,+, cancel) (Reads the "H value" to correspond to the "Height Offset" being applied to the active tool. Typically T22 = H22 = D22)
  • G54-G59 - Work Offset (XYZ location of Program Zero Point, values are typically given "in Machine Coordinates", from the Machine Home Position.)
  • G70-G89 - Canned Cycles (depending on Machine Configuration). Macros to automate repeated motion types (Drilling, Pecking, Tapping, Boring, Reaming, etc.)
  • G90 / G91 - Absolute and Incremental Motion codes
  • G93 / G94 / G95 - Feed Mode (Inverse Time, Units per Minute, Units per Revolution)
  • G98 / G99 - Controls how tools retract after a Canned Cycle Call.

Using Cutter Comp (G41/G42/G40), and TLO (G43/G49), along with Work Offsets (G54, G55, Etc.), allow us to "position a block of stock or work piece anywhere on the machine table", and then we can "tell the machine where the part is located", using a Work Offset. The Cutter Compensation (G41/G42 with a Dxx value), allow us to adjust the "XY size" of the part. We can use different "D Values" (offsets) to control different part features, allowing us to fine-tune the cutting process. TLO allows us to adjust different "depths" on the part, by making slight adjustments to different "height offsets". This allows us to compensate different "part features", by using a unique "TLO" for each feature (potentially), or adjusting "all features" that a tool cuts, by changing a single Height Offset value.

Share this post


Link to post
Share on other sites

Its is a dms 3Axis Router with a fagor 8065 controller. I believe TLO is not setup there are no H values output to the machine it only takes the tool number.

Share this post


Link to post
Share on other sites
5 minutes ago, peter ~ said:

Its is a dms 3Axis Router with a fagor 8065 controller. I believe TLO is not setup there are no H values output to the machine it only takes the tool number.

On the DMS Fagor machine, the tool offset is a single alpha-numeric, D1 if memory serves me correctly. Both height and radius are combined in combination with the #KIN (kinematic offset) parameter.

The Fagor is a very different beast from Fanuc.

  • Like 1

Share this post


Link to post
Share on other sites
2 minutes ago, So not a Guru said:

On the DMS Fagor machine, the tool offset is a single alpha-numeric, D1 if memory serves me correctly. Both height and radius are combined in combination with the #KIN (kinematic offset) parameter.

The Fagor is a very different beast from Fanuc.

Yes I am not a fan. Fanuc controllers are far Superior IMHO.

Share this post


Link to post
Share on other sites
6 minutes ago, peter ~ said:

Yes I am not a fan. Fanuc controllers are far Superior IMHO

I don't know, I am much more comfortable with Fanuc, but once you get used to it, the Fagor has some great qualities.

But given the widespread adoption of Fanuc, I much prefer working with them and their derivatives.

Share this post


Link to post
Share on other sites

I don't know how their 3 axis posts work but our 5 Axis DMS post uses Real Integer #8 to control mid op retracts.  If your is like this try setting #8 to 3 and see if that fixes your problem.  

And on a side note...I've been programming Fanuc and Fagor controls for 10+ years and given a choice I'll take the Fagors any day! (just my $.02 worth) 😀

image.png

Share this post


Link to post
Share on other sites
1 hour ago, jjones61 said:

I don't know how their 3 axis posts work but our 5 Axis DMS post uses Real Integer #8 to control mid op retracts.  If your is like this try setting #8 to 3 and see if that fixes your problem.  

And on a side note...I've been programming Fanuc and Fagor controls for 10+ years and given a choice I'll take the Fagors any day! (just my $.02 worth) 😀

image.png

Thank you for the info!! I will try it when I get back to the office.

Share this post


Link to post
Share on other sites
3 hours ago, peter ~ said:

My Mill page in control def looks like this -->

pic2.bmp

pic1.bmp

So it looks like your post uses Misc #1 to control retracts...I would create a couple of simple contour toolpaths, scroll down to Misc Values for each toolpath and make sure Misc #1 is actually set to 2 then post it and see what the retracts look like. I know sometimes I have to uncheck the "Automatically set to post values" box and manually change the number to make it work right, Also make sure you regenerate the toolpaths before posting them...even if they don't show up as dirty. 

 

1.gif

  • Like 2

Share this post


Link to post
Share on other sites
21 hours ago, jjones61 said:

I don't know how their 3 axis posts work but our 5 Axis DMS post uses Real Integer #8 to control mid op retracts.  If your is like this try setting #8 to 3 and see if that fixes your problem.  

And on a side note...I've been programming Fanuc and Fagor controls for 10+ years and given a choice I'll take the Fagors any day! (just my $.02 worth) 😀

image.png

That looks like a Postabiliy Engine Post.

Share this post


Link to post
Share on other sites
1 hour ago, jjones61 said:

So it looks like your post uses Misc #1 to control retracts...I would create a couple of simple contour toolpaths, scroll down to Misc Values for each toolpath and make sure Misc #1 is actually set to 2 then post it and see what the retracts look like. I know sometimes I have to uncheck the "Automatically set to post values" box and manually change the number to make it work right, Also make sure you regenerate the toolpaths before posting them...even if they don't show up as dirty. 

 

1.gif

 

Looks like the Automatically set to post values was unchecked in some Template operations. I was able to find an affected program and operation once I knew what to look for.  +1 Thank you very much  Jjones and everyone who commented!

Share this post


Link to post
Share on other sites

I confirmed 100 % this was the issue a simple mistake but expensive, would any of you happen to know if this can be updated via edit common parameters?

Share this post


Link to post
Share on other sites
18 minutes ago, peter ~ said:

I confirmed 100 % this was the issue a simple mistake but expensive, would any of you happen to know if this can be updated via edit common parameters?

You can in 2020...I would assume you can in 2018 as well.

 

1A.gif

1B.gif

  • Thanks 1

Share this post


Link to post
Share on other sites
2 hours ago, 5th Axis CGI said:

That looks like a Postabiliy Engine Post.

It Was a Postability post...until I got my grubby little paws on it!  😃

 

  • Like 1

Share this post


Link to post
Share on other sites
25 minutes ago, jjones61 said:

You can in 2020...I would assume you can in 2018 as well.

 

1A.gif

1B.gif

Thank you so much!!! You have no Idea how huge this is for us, we have been bleeding on machine hours.

  • Like 1

Share this post


Link to post
Share on other sites
32 minutes ago, peter ~ said:

Thank you so much!!! You have no Idea how huge this is for us, we have been bleeding on machine hours.

No problem, glad it worked!

I have learned so much from this forum that any time I can help out, I'm glad to do it!

  • Like 1

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us