Shark HD3 Z-axis problems

Discussion/questions about software used with your CNC Shark and programming issues

Moderators: sbk, al wolford

Shark HD3 Z-axis problems

Postby dgarvin » Thu Aug 01, 2019 9:27 am

I have had a CNC Shark HD3 for several years now had experienced issues with the consistency of the Z-axis across a relief cut sign. If I try to flatten the bottom a large pocket, it's like the bit randomly moves up and down and creates something that isn't remotely flat.

The latest problem is actually with a V-Carved sign. I am using a 1/8" upcut spiral to clear the larger pocket area inside the lettering with a 0.1" maximum Z step. The flat depth is 0.1625" so it automatically splits it into two passes. The first cut starts fine on the first letter but as it progresses in the +Y direction, the Z gets higher and higher until it's not even cutting at all on the third letter. The depth measured at the beginning of the first letter is about 0.125". At the end of the second letter (about 3.5" in the +Y direction) the depth is only 0.048"!

This is after redoing the "virtual zero" with the touch plate...several times. According to the control panel (CNC Shark CP V2.1) the maximium difference recorded across a 22" field is about 0.010" so the depth changes while routing should be pretty much undetectable. It's almost like the controller thinks the sign blank is raised up about a lot on the far (+Y) end and compensating for something that isn't there.

Any ideas would be welcome

Dave
Attachments
IMG_20190723_185311504.jpg
Dave

"The right tool can be used for just about anything" - Red Green
dgarvin
 
Posts: 7
Joined: Thu Oct 06, 2016 3:08 pm

Re: Shark HD3 Z-axis problems

Postby dgarvin » Thu Aug 01, 2019 9:40 am

One other issue I encountered was when I was looking to see if there were updates to the CNC shark control panel. The message I got said that the revision available (V 2.1 build 22) may or may not be more recent than the installed revision (V2.1 build 25F). It seems strange to me that the only revision available is older than the revision that I downloaded a year ago.
Dave

"The right tool can be used for just about anything" - Red Green
dgarvin
 
Posts: 7
Joined: Thu Oct 06, 2016 3:08 pm

Re: Shark HD3 Z-axis problems

Postby sharkcutup » Tue Aug 06, 2019 9:39 am

Just out of curiosity

Have you checked recently if that the machine gantry (z-axis) is still true to the machine bed in both the z-axis and the y-axis?
I am suspecting either the z-axis & gantry is not true to the x and y axis or your material board is not planed true (varying thicknesses). I periodically check my machine for this especially if I am going to carve an intricate 3D carving such as an Aztec calendar or a Marvel comics calendar both of which have a lot of V-carving throughout.

I have virtual zero on my machine with a .375" thick touch plate. I use it extensively for 3D carvings and in some cases 2D especially in case where text is being used. I have not seen anything like what you are having.

Is there a way you could post your .crv file for review here on the forum provided there are no copyright materials (3D models n such)? Looks as if it may be more of a machine problem but just want to be able to get a ruling on the V-Carve file to be sure there are no issues there that may be adding to the discrepancy noted.

Sharkcutup
Last edited by sharkcutup on Tue Aug 06, 2019 12:30 pm, edited 1 time in total.
Shark HD3 Pro Plus Extended Bed with Water-Cooled Spindle
Facebook: hoganscnccrafts.com
sharkcutup
 
Posts: 341
Joined: Tue Mar 08, 2016 5:23 pm

Re: Shark HD3 Z-axis problems

Postby Bob » Tue Aug 06, 2019 10:50 am

Dave,
I have three questions:
1 is the gantry changing Z when it shouldn't?
2. Is the router slipping within the clamp?
3. Is the router bit slipping within the collet?
And, a fourth:
4. Is there anything on the table that is changing heights?

Bob
User avatar
Bob
 
Posts: 1116
Joined: Sun Aug 08, 2010 3:35 pm

Re: Shark HD3 Z-axis problems

Postby dgarvin » Wed Aug 07, 2019 9:22 am

@sharkcutup The files are attached.

@Bob
Nothing on the machine is moving that shouldn't. If I rerun the same file twice, it makes the exact same cuts twice.

I did a few experiments with some pieces of MDF and a 1-1/2" surfacing bit and I'll put the results here when I get some pictures. The three experiments were:

Machine: CNC Shark HD3 with water cooled spindle
Bit: 1-1/2" planing bit
V-Carve Desktop 9.5
Shark control panel V2.1 B.25f
Material size approximately 6.5" x 6.5"
Cut depth = 0.030"

#1 Moving spindle using the "jog" feature in the control panel...
Mill the surface starting in the lower left corner and move +X.
Move completely back to the starting point, shift +Y by 1.2" and make another cut.
Repeat for rest of the material surface.

#2 Moving spindle using tap file with virtual zero disabled...
Created a pocket cut 7" x 7" and saved the tap file (Horizontal raster, 80% step over)
Ran the tap file after using the touch plate on the material surface

#3
Same as #2 with virtual zero enabled

All of the results were pretty much the same with the virtual zero case slightly worse. With all three of these tests, it became evident that there were two related issues.
1. The spindle is not perfectly perpendicular to the x/y plane but it is probably shifted in the clamp. There was a bit of "clapboard" effect where it leaves a ridge of about 0.006" between one pass and the next.
2. The x/y plane is not perfect either. There is about 0.012" difference between X,Y = 6.5",0 and X,Y = 0,6.5".

While these are troubling, they don't add up to the problem I was seeing with the pocket cut with an 0.125" end mill. I've seen a few of these complaints in past forum posts and they all seem to be with a 1/8" or smaller end mill. Maybe there's something there? A scaling issue with the virtual zero planarity calculation with small bits on a large field?

I plan on repeating this experiment on a pocket cut with a small bit when I'm done with my day job. Stay tuned...

Dave
Attachments
V-Carve 1.tap
V-carve tap file
(151.04 KiB) Downloaded 26 times
V-Carve 1 [Pocket].tap
Clearing tap file
(175.17 KiB) Downloaded 25 times
hygge4.crv
Design file
(1.14 MiB) Downloaded 27 times
Dave

"The right tool can be used for just about anything" - Red Green
dgarvin
 
Posts: 7
Joined: Thu Oct 06, 2016 3:08 pm

Re: Shark HD3 Z-axis problems

Postby sharkcutup » Wed Aug 07, 2019 11:20 am

I noticed in both your .tap files that the Post Processor you have choosen creates the G64 to a setting of P .01 which is a tolerance setting. Most people edit or create a new the post processor changing this to a tighter tolerance. In fact I had changed my Post Processors to a setting of G64 P.001

I also noticed that the .tap file is directly from the post processor - Correct? It does not have any corrections for Virtual Zero on the Z-axis.

Do you have a copy of your .tap file After the Virtual Zero Corrections are applied?

Sharkcutup
Shark HD3 Pro Plus Extended Bed with Water-Cooled Spindle
Facebook: hoganscnccrafts.com
sharkcutup
 
Posts: 341
Joined: Tue Mar 08, 2016 5:23 pm

Re: Shark HD3 Z-axis problems

Postby dgarvin » Wed Aug 07, 2019 12:32 pm

I have never looked into editing the post processor. Is there a defaults file that it pulls this information from, or is the post processor itself a text file that can be edited? I always assumed that it was some compiled object and have never gone looking for it. What directory would that be stored in?

How do I get the file after virtual zero adjustments are made? Can that be saved from the control panel? That would probably have all the answers I'm looking for right there. I'm not an expert in G-code but you can bet your boots I'm going to be coming up to speed pretty soon. This issue has annoyed me long enough.
Dave

"The right tool can be used for just about anything" - Red Green
dgarvin
 
Posts: 7
Joined: Thu Oct 06, 2016 3:08 pm

Re: Shark HD3 Z-axis problems

Postby sharkcutup » Wed Aug 07, 2019 4:57 pm

The Post Processor & Tool Database (default files) and several other necessary files are located in the location I am about to describe/tell you about.

Open V-Carve to first screen (it is also on the other fully opened with job screen too)
Select file (upper left) then Open Application Data Folder
Here you will notice two things in particular
1.) the location as stored in your computer (first line at top of pop-up box)
2.) All the necessary data files for V-Carve (in particular the Post Processor & Tool Database) there are others there of interest too but for now those two a rather important.

It it recommended that you create a backup copy stored in another place on your computer of those two directories as a minimum!

The Post Processor and/or the .tap files can be edited using notepad or any text editor.

Hope This Helps!
Sharkcutup
Shark HD3 Pro Plus Extended Bed with Water-Cooled Spindle
Facebook: hoganscnccrafts.com
sharkcutup
 
Posts: 341
Joined: Tue Mar 08, 2016 5:23 pm

Re: Shark HD3 Z-axis problems

Postby jeb2cav » Wed Aug 07, 2019 5:19 pm

Hi Dave,

Some additional thoughts after entering the conversation at this point - from your very first picture - having a ~0.35" difference in pocket depth is frankly either a rogue virtual zero setup (somehow) or you have a mechanical issue of some sort (that may be hard to recognize). If you have any slop at all, you may want to try loosening the z axis coupler, getting it all 'tight', and then tightening it and trying again. I would frankly run with without a virtual zero workflow for a starting sense of the mechanical condition. Could be a burr along the spiral rod as well - or a hard bit of material on the lead screw.

On the G64 - the easiest thing to do would be to open the tap file using notepad (as discussed) and setting that to P0 - and running at a low tool path speed as well - until you are able to narrow this down.

To add to some of the discussion - there is an old pdf on the post processors, some of which is still applicable - https://docs.wixstatic.com/ugd/59d161_2fbe0591b8ad40cfba1607a0e0f1922c.pdf - and if you go down to page 8 and 9, you can see the discussion on this setting. As pointed out, you can create your own custom post processor to use in generating the tap file.

I would take the file you ran for the picture in your first post, edit G64 to P0, run at a very slow IPM (either in the tap file or using the slider to slow the machine down) and go from there. Again, I can't imagine that your table is 0.35" 'off' over 3.5 inches. Bob's questions I suspect were based on similar thinking of a mechanical challenge of some sort.

As you stated, you may also be out of alignment between the gantry and the table as well. While that would aggravate this in a pocket, you should still have a similar depth of cut over 3.5".

You mention in a later post you were getting a ridge of about 0.006" between passes. That is within the G64 P0.01 setting.
jeb2cav
Site Admin
 
Posts: 1527
Joined: Thu Sep 30, 2010 7:04 pm
Location: Kentucky

Re: Shark HD3 Z-axis problems

Postby sharkcutup » Wed Aug 07, 2019 6:21 pm

How do I get the file after virtual zero adjustments are made? Can that be saved from the control panel? That would probably have all the answers I'm looking for right there. I'm not an expert in G-code but you can bet your boots I'm going to be coming up to speed pretty soon. This issue has annoyed me long enough.
dgarvin asked

Not exactly sure how to get that file but it can be viewed using the View menu (upper left) and select View Virtual GCode in the control panel software. Probably could go to a portion of interest and shoot a photo of it and then upload/post the photo here. Maybe someone out there can enlighten us as to how to get the GCode file with the Virtual Zero readings. I have never really had a problem with Virtual Zero so I never had to venture there.

On another interesting note to take into consideration in the Preferences under Virtual Zero on the Control Panel software there is a Section named Collection points. Here there are two selections Material Edge and Image Cutting Area. These should be changed depending the actual data collection area required for Virtual Zero on the individual carving circumstances.

Just some more Thoughts to Comprehend!!!

Sharkcutup
Shark HD3 Pro Plus Extended Bed with Water-Cooled Spindle
Facebook: hoganscnccrafts.com
sharkcutup
 
Posts: 341
Joined: Tue Mar 08, 2016 5:23 pm

Next

Return to Software. Programming

Who is online

Users browsing this forum: No registered users and 2 guests

cron