Rough and Finish pass not matching toolpath!

[farmertom]

Hi,
Either I am having a problem with the rough and finish tool paths creation or i don't understand something.

The first two images are of the left side and right side of a project I am working on. The images show the
edges of where the rough and finish toolpaths have made cuts.

The third and fourth pictures show the same areas but I have included images from Aspire showing the tool pathes
and the 2D view showing the rectangular vector used to limit the tool paths and the edge of the elephant object.

What I have done is place a rectangular vector around the 3D objects to limit (or extend) the tool path cuts. I
wanted the elephants to be in a "Shadow Box". After the rough cut pass I used the same vector to make a profile
cut (on line) to trim up the "waves" made by the bits on the end grain.That appears to have completed
successfully. Then proceeded with the finish pass.

As you can see the cuts in the project do not match the tool path as shown in Aspire. Both the rough and finish
cuts are not ending in the same place as indicated in the Aspire image. The Image generated by Aspire in the tool
path preview does not show this also. This has happen to me on other projects also.

My CNC machine is not losing steps because the 3D elephants are not malformed.

So, What am i missing!

[rej]

here is another way

click on your elephant, then click on the icon to put a boundary around it.
now select the elephant boundary and run your finish pass toolpath. (in preview mode)
now select the rectangle and the elephant boundary, and run a pocket toolpath. set a depth, and change that depth until it looks good around the finish pass.

then cut the pocket first and then cut the elephant. probably won't need a roughing pass.

[tmerrill]

I'm having a hard time seeing how what was actually cut was the same toolpath generated using the Aspire previews you show.

When I duplicate your steps (with the exception of the profile pass to clean up the edge) the corners are more square than what you got which agrees with the toolpath preview pictures you show.

Are you sure the cut files saved and used are the right ones?

Tim

[farmertom]

I'm having a hard time seeing how what was actually cut was the same toolpath generated using the Aspire previews you show.

When I duplicate your steps (with the exception of the profile pass to clean up the edge) the corners are more square than what you got which agrees with the toolpath preview pictures you show.

Are you sure the cut files saved and used are the right ones?

Tim

Yes, I am sure that the cut file is the same one I used and taking the pictures from. I agree, The aspire file looks fine. I saved the gcode to a file and loaded it into Mach3 to cut. I can't explain it unless Mach3 has something to do with it. Attached are two images from Aspire. The first is a preview, the second is the same preview with the rough, profile and finish pass. I have added pictures of the completed project. What could cause the edges of the finish pass to do that?

[tmerrill]

I used a 1/4" end mill for the rough, 1/8" ball nose for the finish.

If that is the preview you are seeing in Aspire and not getting it at the machine, then you need to look at the machine or it's control system. I'm happy you told us it was Mach 3 as there are a lot of posts on here about how different settings can affect the results. I'll let someone with Mach 3 experience help you with that.

As for everything you did in Aspire, it all looks great.

Tim

[farmertom]

I used a 1/4" end mill for the rough, 1/8" ball nose for the finish.

If that is the preview you are seeing in Aspire and not getting it at the machine, then you need to look at the machine or it's control system. I'm happy you told us it was Mach 3 as there are a lot of posts on here about how different settings can affect the results. I'll let someone with Mach 3 experience help you with that.

As for everything you did in Aspire, it all looks great.

Tim

Tim,
Please look at my earlier post, I add some images of the completed project. Do you think Mach3 could to that to the end of a run and not screw up somewhere else?

[rdean33422]

Could you please post a copy of the .crv file for us to examine.

Thank you

Ray

[tmerrill]

No file can be posted that contains that 3D Model or toolpaths to recreate it.

As for the preview question, I'm only saying that if the preview in Aspire looks good, it is not an Aspire issue. That leaves the post processor, machine, control system, setup or a combination of them. Since there have been many posts regarding Mach3 settings, I would suggest you start there.

Tim

[esteeme1]

Tim,

John's file is not the same as yours and it appears to be modeled at home. Have you seen his file for sale somewhere? It's an elephant.

[tmerrill]

Yes, I saw that after I posted - just reacted to someone who apparently doesn't have Aspire requesting the (wrong type of) file.

If it is a file that can be shared (for sure), that is fine. However, since the Aspire preview looks fine I can't see what value looking at the file will have.

He is using a raster strategy for both rough and finish toolpaths, the center part is cutting fine and the problem seems to come at the start and finish of the raster passes where acceleration/decleration is in effect. If you look closly, the ridge he is getting at the sides is straight and parallel to the sides at the top and bottom where there is no model present and loosely follows the shape of the elephant where that is present.

I'm surprised that none of the Mach3 users have offered suggestions, or even saying there was nothing in Mach3 that would affect this would help.

Tim

[esteeme1]

Considering Mach3 the only question I can think to ask is; What does the preview look like in mach3? Also I see a carvewright in the background, I wasn't aware that the machine could interface with mach3. Could the toolpath be calculated with the wrong PP?

Edit: Ok maybe that's a planer.

[kilrabit]

Farmertom,

Can you tell me you speeds and feeds? It looks like either you are going too fast, or you accelleration is too little. Also check and make sure that your tool setup does not accidentaly have mm per minute and you are running inches per minute.




Roy

[esteeme1]

Roy,

I think you may be on to something. I'm wondering if the axis acceleration speeds are equal to each other. My thought is, if you look at the roughing pass the stop point is at the same point and there isn't a height variation with the roughing pass. With the finish pass the length of cut seems to coincide with height variance. If it isn’t the acceleration factor make sure that the turns per inch / mm are set correctly in all axes. If it isn't tuning than make sure the scale factor for each axes are equal.

[farmertom]

Hi,
I want to catch up on all of the reply posts.

The elephant is some what home grown. I downloaded a line drawing from the web and used the create shape tool to make it 3D. If the line drawing is copyrighted, does that keep me from giving away my elephant? I still needs a little work.

All settings are OK as far as mm vs. inches, etc.

That is my Delta 12 inch planer in the background. I will attach a photo of my DIY machine.

Rough pass is 120 IPM with a 1/4 upcut end mill running at 13K RPM and 0.2 inch cut depth, 40% step over.
Finish pass is 200 IPM with 1/8 ball nose running at 10K, general depth is 0.040 inches with 10% steo over.

I did a little testing by making some "air cuts" last night. I observed in the graphic view if Mach3 has the CV turned OFF the end mill appears to travel to the end of the toolpath raster. If the CV is turn ON the endmill appears to stop short of the tool path raster. I need to confirm this with some actual cuts. I will do that as soon as i can.

Can someone explain the CV parameters and how that effects changes the toolpath and recommend setting in Mach3?
Thanks for your help and suggestions

farmertom
http://cncartwork.weebly.com/index.html

[esteeme1]

CV, when selected the program makes every attempt to keep the cutter moving forward it will change the speed of advance while the cutter changes height but will continue to move forward. This setting shouldn't affect the stop point of the toolpath it should continue to move forward to the proper end point. The program doesn't know where the cutter head is and believes it has reached the correct stopping location. So my thought with your issue is it's possible that your seeds or turns per inch are not meshing in each axes of your setup/configuration/motor tuning. As I look closer it doesn't appear as if you're losing steps either so I start to think motor tuning all over again. So what I think is happening is that your Z axis is moving to the elevation point fast than the x axis thinks it is. At the end of the run X stops short or it may be Y in your case (either way). That would be my guess as to why it stops short with no elevation change as well.

Exact Stops setting is just that the cutter will reach the exact point of the elevation change in other words move to each point in the tool path.

Here is a link to the Artsoft explanation of CV
http://www.artsoftcontrols.com/docs/Mac ... ngs_v2.pdf

edit: X or Y is stopping short because of turns per in calibration/motor tuning with no elevation change and has an extended run because z is moving fast than the program believes or is not calibrated.