[peteeng]

Evening all - especially any post gurus. I'm deconstructing this post and trying to make the first move a clearance height move. Any suggestions would be helpful as I may take a while to figure it out.

Image "first move" is the output of the post. I want the first move to be to the clearance ht not across the part then up.
Scoot Post No1 is the post that produced this code

Peter

[mactec54]

Evening all - especially any post gurus. I'm deconstructing this post and trying to make the first move a clearance height move. Any suggestions would be helpful as I may take a while to figure it out.

Image "first move" is the output of the post. I want the first move to be to the clearance ht not across the part then up.
Scoot Post No1 is the post that produced this code

Peter

Your Z move is already at G53G0Z0 at the top of the start of the program, if you have homed your machine, so it is fine as posted the Z axis should be up which it is, then the X Y can move then the Z axis can come down to the G1Z17F___. this can be a rapid G0 move, or a G1 Feed move so you don't have to change it from what it is

[peteeng]

Hi Mactec - My usual procedure is to zero the tool relative to the part and start there. This has always worked when I program via UCCNC CAM its first move is always to its safe ht. But I can see that I can zero the tool then manually raise to the "home" or clearance ht and then start. Easily done and seems that's the correct way to do it. . My machines don't have homing switches been on the list for years but haven't got to do it yet. Maybe do it on Matts machine... Thanks to all for the insights. Peter

[LorenBMS]

A question for the F360 CAM gurus. I often clamp the RHS cut the LHS reclamp LHS cut RHS for profiles. But in F360 I can't seem to figure how to path this. Do I have to make dummy geometry? If I use edges or sketch's the tool goes down the middle and I can't find an instruction for inside or outside of the line?? In a wireframe modeler this is easy. Seems I have to make a dummy LHS and RHS so F360 can figure it out... Hmmm Peter

Peter, In F360 you can create sketch geometry to control CAM tool paths. For example the first image I have a sketch on the left half of the part profile and selected in in a 2D contour tool path. The red arrow is selectable and it flips the path from the outside to the inside of the tool path line. The 2D tool paths do not seem to recognize the solid, so the red arrow is used. The second image shows a second sketch on the right half of the profile to use for the next tool path.

The third image shows using a sketch on top of the part use to limit the area machined by a 3D adaptive path to clear out just the pocket inside of the selected sketch and not the whole part.

Using sketches to control the tool paths is a powerful tool in F360.

[peteeng]

Hi Loren,
Thanks for that, I shall work on it. My fusion machine just had a video driver hiccup with a dreaded blue screen error. So its off to the tech. I'll try to load F360 on this machine. Looks straight forward. Thanks for the info. Similar to Mecsoft (and others I suppose) Peter

[mactec54]

Hi Mactec - My usual procedure is to zero the tool relative to the part and start there. This has always worked when I program via UCCNC CAM its first move is always to its safe ht. But I can see that I can zero the tool then manually raise to the "home" or clearance ht and then start. Easily done and seems that's the correct way to do it. . My machines don't have homing switches been on the list for years but haven't got to do it yet. Maybe do it on Matts machine... Thanks to all for the insights. Peter

Then that first move G53G0Z____ needs to be a number that is going to clear everything which could be anything like 50 having it Zero will crash into something, there is no point in having it in the program if it is not doing its job.

Not having homing switches, you are not serious about your machine builds, as this is an important part of any CNC machine, this is always a crash waiting to happen as the control will never know where an Axis is relative to the machine's max travels

[peteeng]

Hi Mactec - That gets us back to my first question. The G53 is created by the post so I can't leave it out unless I mod the post. Or manually edit the code. I've noted to you before I build Maker grade machines which are very cost sensitive so anything that is not "absolutely " necessary is left out. The Maker or builder can add these as they go. I get along fine without them. The occasional crash is generally due to fixtures more than motion limits. On another topic I have been trialling an epoxy used for casting that takes days to cure. Its extremely thin and will seep under masking tape and through timber really well. I expect it will be ideal for EG and can be used in the dry fill then pour technique. It will be excellent for infusing carbon fibre as some types of CF cloth are hard to infuse even with infusion resins. I post cure at 40C for two days and it becomes very hard and sands very well. It is also exceptionally clear. For those in OZ interested look at Luci-Clear

https://boatcraft.com.au/information...waApE3EALw_wcB

Was very disconcerting the first time I used it for fill some large holes in a timber slab. At 24hrs it was still pourable, at 48hrs was gummy but 36hrs was hard. Its around 18-20deg C here at the moment thru the day. So I used it in a smaller job that I could put in my oven, and set it at 30C. 2 days and its extremely hard and clear. So now I'd better make some CF or composite parts. Peter

[joeavaerage]

Hi,
I use Fusion 360 and Mach4. Fusion has a Mach4 post. Amongst the top level choices you can make is the section called Clearance Height. See attached.
If youuse the option called 'Clearance Height' the actual heights you nominate when you compose the toolpath. If you use some of the other options
thats when you find calls like g28, g30 g53 etc.

This applies to the Fusion Mach3 and Fusion Mach4 post....I cant see why it would not be included in a UCCNC post.

Craig

[joeavaerage]

Hi,
just had a look and the Fusion UCCNC post it a little different but includes the option 'Clearance Height'.

Craig

[mactec54]

Hi,
just had a look and the Fusion UCCNC post it a little different but includes the option 'Clearance Height'.

Craig

Yes, that's all he needs to use is a clearance number in there and he is good to go with no editing to do

[joeavaerage]

Hi Peter,
if you use the 'Clearance Height' option in the post then you can define things like Retract Height, Clearance Height, Bottom Height from defined planes of your model, maybe the Stock Height
or the Model Top. You can assign an offset relative to that plane or planes. All the retracts are performed relative to the job you are doing and do not depend on the machine.

Craig

[peteeng]

Hi Al - Thanks for the input. The bottom ht top ht retract ht clearance ht and safe ht can all be speced in the Fusion CAM setup, plus the clearance can be modified in the post setting. However the issue for me has been my procedure not the post as I do not have a home position. So now I set up (0,0,0) on the part move Z up to the required safe ht. and set the UCCNC safe ht to the same safe ht so there's no conflict out of program. . That covers the bases so far. I did a test part along those lines today and it worked well. My computer with fusion had a video card failure yesterday and its at the techs shop. Just got word its fixed and I can pick it up tomorrow. I shall load fusion onto the workshop machine so I can do mods on the fly and check the new procedure asap. I wanted to do a LHS-RHS part with fusion but had to do it the old way in Rhino today. Thanks for all the input I'll wade through it slowly. Matt wants home/limit switches on his Scoot so we'll work thru that together as well. If the cables arrive before Friday we may have motion this week!! Thanks again Peter

[mactec54]

Hi Al - Thanks for the input. The bottom ht top ht retract ht clearance ht and safe ht can all be speced in the Fusion CAM setup, plus the clearance can be modified in the post setting. However the issue for me has been my procedure not the post as I do not have a home position. So now I set up (0,0,0) on the part move Z up to the required safe ht. and set the UCCNC safe ht to the same safe ht so there's no conflict out of program. . That covers the bases so far. I did a test part along those lines today and it worked well. My computer with fusion had a video card failure yesterday and its at the techs shop. Just got word its fixed and I can pick it up tomorrow. I shall load fusion onto the workshop machine so I can do mods on the fly and check the new procedure asap. I wanted to do a LHS-RHS part with fusion but had to do it the old way in Rhino today. Thanks for all the input I'll wade through it slowly. Matt wants home/limit switches on his Scoot so we'll work thru that together as well. If the cables arrive before Friday we may have motion this week!! Thanks again Peter

No, you are missing the point completely, the Z setting for the G53G0Z___ will work with you setting your part Zero off your work this is one of the most important moves that is in you program as it is the first axis move

You need to put your clearance number in this first Axis move, you have it at Zero this needs a number and then you will have safe machine movement set it to say 50 then start you program in Single Block, and every time you press the start Button you will see what each line of code is doing.

Do the test above after you have set your tool to the top of your work, the first move than should have the Tool 50mm above the Part, if it has been setup correctly.

[peteeng]

Hi Mactec - I have the clearance ht set at 30mm in the cam set up and the post makes it Z0. I shall check to see if the cam set up and post are in conflict when I get my computer back. Maybe the post properties overrides the cam setup...Peter

[peteeng]

Good afternoon Gentlemen and Ladies - I have picked up my computer so now can look at Fusion again. I picked a part and set up the heights as per image. This means the clearance ht is 22mm. In the simulation side of things it all works as the tool starts at the path start (not at 0,0,0). When it comes to posting the code there are two options under the "safe retract" menu 1) G53 and 2) clearance ht. See the code difference for each selection (post compare image)

In UCCNC general settings I have set the safe Z height to 20mm

So if I run the G53 code and I start at (0,0,0) as per my usual procedure the tool stays at Z0 and moves across to the path start
If I run the clearance ht code it does the same.

So the takeaway is not to start at (0,0,0) but at the Z clearance ht or at a nominal "home" ht and use the clearance ht setting in the post. If the G53 is used it will move down to Z0 from the home position then across the part then up to the path start. I'm now clear about the whys and wherefores so thanks for the input as usual.... Peter

[pippin88]

Peter, unfortunately I don't think you are clear.

On mobile so can't type a full guide.

You need to have a look at:
World Coordinates (G53)
Work offsets (G54-G59, most commonly G59).

The machine needs to know where it is in space (world coordinates)
The easiest way is with home switches. You home the machine, it knows where it is, and will not exceed the specified travel limits (sometimes called soft limits)

Without home switches, you still need to home the machine, but this is usually done by manually jogging to the correct position (roughly near the edge of travel) and homing or zeroing the machine (terminology may vary)

Then after the machine knows where it is in space, you tell it where the work is (work offset, usually G54). This is usually done by jogging each axis to the correct spot and touching off / zeroing that axis (terminology varies).
You will then be working in work coordinates.

If G0 G53 Z0 sends the tool tip down to the work surface, then you have told the controller that is where Z0 is in machine space.

The convention is that G53 (machine coordinates) Z0 is full up (on a standard 3 axis machine). G53 Z0 should be a safe height to make X and Y moves with any length tool.
(For work coordinates, G54 Z0 is often set as top of material but can also easily be bottom of material / top of spoilboard, depends on preference and situation)


Having home switches allows you to recover from power failure, reduces crashes and stuff ups and makes life easier.

[pippin88]

The clearance G code you've posted does not have any 'safe Z' move to start with. The first moves are in X and Y.
The first Z move is Z22, after an X and Y move.

It's usually a good idea to have a safe Z move as the first thing. Reduces stuff ups!

[peteeng]

Hi Pippin,
The "safe move" you recommend is my original question. I'm looking at the post to try to introduce that automatically. But starting at a nominal home Z practically is the same thing. I appreciate the commentary about homing switches but most (99%) of the machines I get to look at don't have them they are Maker grade machines (if thats a class). Like today a guy showed up with a $400 Chinese engraver looking for advice...

So the whole conversation has to understand that I'm coming from a machine and code that does not home. I also appreciate learning what the conventions are in operating cncs as I'm self taught so will have bad habits.

UCCNC has machine co-ords which I expect are world co-ords. And work co-ords. I usually move the tool to the decided (0,0,0) and zero the machine and work co-ords. When importing a dxf and generating code UCCNC always uses a safe Z ht first move. When using mecsoft I always move the CAD model so the desired machine 0,0,0 is where I want the tool 0,0,0 to be. Then post the code then set the tool to the part. Then its all OK to go. Posting in fusion I have to deal with it a bit different. I'm happy with my current procedure and I think it mirrors the procedure if it had a home. I'll look at soft limits to see how they fit in as well.... Big subject difficult to describe in a few sentences.... Thanks to all for the input my understanding is getting better.

I will run a few test codes to check fusions behavior with my new procedure...Peter

I notice that the new screen of UCCNC displays work co-ords and machine co-ords simultaneously maybe they picked up that the original display needed a bit more info?

[pippin88]

The reason you are having G53 Z0 issues is that your world/machine coordinates (G53) and your work coordinates/work offset (G54) are the same.

Based on the examples you posted, you can use the 'clearance height' option in Fusion. It will not move the Z down to Z0. But it will also not doing any move up to a safe Z before starting to move in X and Y.
You must remember to move Z up after zeroing.

There is no G Code for retract height / clearance height / safe Z.
This is because there is no way for a controller to know height of any clamps/protrusions/workpiece etc. And you have to deal with tool length etc.

For single spindle manual tool change machines (like yours) you should not bother with tool length offsets. You don't have any set tool lengths.

There is a big difference between hobby CAM, such as Vectric, and CAM designed for professional use. Using professional CAM for hobby use can be a pain as often things like automatic tool changers and tool tables with tool lengths etc are expected. (I haven't really used Fusion.)


As a hobbyist, I would immediately rule out buying any machine that did not have home and limit switches.
I know you have to compete, but dodgy machines built to minimum price which result in much hair pulling and complaints on online forums should not be what you are aiming to match!

[peteeng]

Hi Pippin - It's easy for the Maker to add these things and they do. They all have different approaches to machining and different software (or none) My aim is to provide a base that they can all move off from in confidence. Which they do. I have shown lots of people how to use UCCNC via dxf and they get along fine, I speak to people with no machining background who are using fusion and they are doing OK as well. My machines are not minimum price and I'm confident they provide a very good machine at a budget price. Thanks for the interest and input. The clearance ht setting is my current preferred route for the Fusion post which removes the G53 issue. Peter