SA International Forum Homepage
Forum Home Forum Home > EnRoute FAMILY > General EnRoute
  New Posts New Posts RSS Feed - possible bug
  FAQ FAQ  Forum Search   Events   Register Register  Login Login

possible bug

 Post Reply Post Reply Page  12>
Author
Message
PlastecProfiles11 View Drop Down
Master
Master
Avatar

Joined: 04 May 2015
Location: United States
Points: 160
Post Options Post Options   Thanks (0) Thanks(0)   Quote PlastecProfiles11 Quote  Post ReplyReply Direct Link To This Post Topic: possible bug
    Posted: 11 July 2016 at 2:30pm
In Enroute 5 when I do a Island fill and put a 90 deg. conic to put a bevel on outside of that and put the conic in 2 passes it doesnt line up the conic in the corner.
Learn to automate Enroute by seeing an example at https://github.com/PlastecProfiles/EnrouteAddin
Back to Top
Stewey View Drop Down
Professional
Professional


Joined: 07 May 2008
Location: Australia
Points: 93
Post Options Post Options   Thanks (0) Thanks(0)   Quote Stewey Quote  Post ReplyReply Direct Link To This Post Posted: 15 July 2016 at 6:29pm
Is the geometry of your cutter perhaps not a perfect 90 degrees (eg 89.5 deg) ? Or  perhaps the spindle head isn't totally 90deg to the bed in both directions?

Is it ALL two-pass cutting with that cutter that doesn't line up smoothly? A photo might help?

(alternately, you can ignore this comment as I don't have ER5!)  ;)

Back to Top
PlastecProfiles11 View Drop Down
Master
Master
Avatar

Joined: 04 May 2015
Location: United States
Points: 160
Post Options Post Options   Thanks (0) Thanks(0)   Quote PlastecProfiles11 Quote  Post ReplyReply Direct Link To This Post Posted: 18 July 2016 at 12:48pm
It is only on the corners it is not the bit because on the rest it was perfect.
Learn to automate Enroute by seeing an example at https://github.com/PlastecProfiles/EnrouteAddin
Back to Top
Todd Zuercher View Drop Down
Master
Master


Joined: 16 April 2010
Location: United States
Points: 145
Post Options Post Options   Thanks (0) Thanks(0)   Quote Todd Zuercher Quote  Post ReplyReply Direct Link To This Post Posted: 11 August 2016 at 8:49am
Have you looked at your g-code with Backplot (look in the Solutions pull down menu) to check to see if the problem is in the file or if it is a problem with your machine.

If the passes all line up right in Backplot, then it is a problem with your machine (backlash, slop, flex, lost steps...)
Back to Top
PlastecProfiles11 View Drop Down
Master
Master
Avatar

Joined: 04 May 2015
Location: United States
Points: 160
Post Options Post Options   Thanks (0) Thanks(0)   Quote PlastecProfiles11 Quote  Post ReplyReply Direct Link To This Post Posted: 11 August 2016 at 12:28pm
They do not line up.
Learn to automate Enroute by seeing an example at https://github.com/PlastecProfiles/EnrouteAddin
Back to Top
PlastecProfiles11 View Drop Down
Master
Master
Avatar

Joined: 04 May 2015
Location: United States
Points: 160
Post Options Post Options   Thanks (0) Thanks(0)   Quote PlastecProfiles11 Quote  Post ReplyReply Direct Link To This Post Posted: 11 August 2016 at 5:15pm
If you try this you will see the conic toolpath does not up in the corner like it does on the regular engrave. I think that is the problem.
Learn to automate Enroute by seeing an example at https://github.com/PlastecProfiles/EnrouteAddin
Back to Top
Todd Zuercher View Drop Down
Master
Master


Joined: 16 April 2010
Location: United States
Points: 145
Post Options Post Options   Thanks (0) Thanks(0)   Quote Todd Zuercher Quote  Post ReplyReply Direct Link To This Post Posted: 12 August 2016 at 11:20am
I think I might see what you mean.  Are you wanting the conical bit to make a square inside corner when using it on a female offset path the same as when using it for an engraving tool path?  And when you set the offset path for 2 passes the point of the first pass gouges the inside corner radius at the top of the 2nd pass.  The 1st path should cut a radius at the corner rather than a square corner.  I've seen this problem before and just considered it the nature of the beast, there are ways to work around it without too much difficulty.  One is to use the engraving path (if you want a square corner).  If you want the conical inside radius, there are a couple of ways to make it work, one would be to explicitly draw the tool paths for each pass (use the offset tool to draw the final pass, then draw the first pass as an offset of that (using round corners)
Back to Top
PlastecProfiles11 View Drop Down
Master
Master
Avatar

Joined: 04 May 2015
Location: United States
Points: 160
Post Options Post Options   Thanks (0) Thanks(0)   Quote PlastecProfiles11 Quote  Post ReplyReply Direct Link To This Post Posted: 12 August 2016 at 11:47am
Yea that sounds like you got what I was saying. And yea that work around would work well.
Learn to automate Enroute by seeing an example at https://github.com/PlastecProfiles/EnrouteAddin
Back to Top
Todd Zuercher View Drop Down
Master
Master


Joined: 16 April 2010
Location: United States
Points: 145
Post Options Post Options   Thanks (0) Thanks(0)   Quote Todd Zuercher Quote  Post ReplyReply Direct Link To This Post Posted: 12 August 2016 at 12:25pm
An even better work around is to add a radius to your inside corners equal to the depth of your bevel cut (for a 90 deg bit).  The final pass will have the square corner and the 1st pass (and any inbetween) will have the correct radius.
Back to Top
Todd Zuercher View Drop Down
Master
Master


Joined: 16 April 2010
Location: United States
Points: 145
Post Options Post Options   Thanks (0) Thanks(0)   Quote Todd Zuercher Quote  Post ReplyReply Direct Link To This Post Posted: 12 August 2016 at 12:50pm
like this
https://postimg.org/image/an7kc0zjf/
Back to Top
PlastecProfiles11 View Drop Down
Master
Master
Avatar

Joined: 04 May 2015
Location: United States
Points: 160
Post Options Post Options   Thanks (0) Thanks(0)   Quote PlastecProfiles11 Quote  Post ReplyReply Direct Link To This Post Posted: 15 August 2016 at 8:04am
Genius!!
Learn to automate Enroute by seeing an example at https://github.com/PlastecProfiles/EnrouteAddin
Back to Top
PlastecProfiles11 View Drop Down
Master
Master
Avatar

Joined: 04 May 2015
Location: United States
Points: 160
Post Options Post Options   Thanks (0) Thanks(0)   Quote PlastecProfiles11 Quote  Post ReplyReply Direct Link To This Post Posted: 16 August 2016 at 12:28pm
Did you all ever have trouble with entries on an offset with a width that is wider than the bit?
I found that it simply will not put one on. The workaround is that you put an angle on that is over 20 degrees. I tried a 10 degree angle but that didn't work. 
Learn to automate Enroute by seeing an example at https://github.com/PlastecProfiles/EnrouteAddin
Back to Top
paloalto_17 View Drop Down
Admin Group
Admin Group


Joined: 29 October 2012
Location: United States
Points: 233
Post Options Post Options   Thanks (0) Thanks(0)   Quote paloalto_17 Quote  Post ReplyReply Direct Link To This Post Posted: 16 August 2016 at 12:51pm
I just want to clarify but your saying that if you have a 1/2 inch End mill for example and you do a routing offset, then you choose .75 in the width of cut, and you also choose a line entry with 3D line checked you are not getting a Entry on the toolpath?

If this is what you are referring to I can look into it and see if there is an issue there. 

Best regards, 
Aaron
Back to Top
PlastecProfiles11 View Drop Down
Master
Master
Avatar

Joined: 04 May 2015
Location: United States
Points: 160
Post Options Post Options   Thanks (0) Thanks(0)   Quote PlastecProfiles11 Quote  Post ReplyReply Direct Link To This Post Posted: 16 August 2016 at 4:29pm
Yes that is what I am referring too.
Learn to automate Enroute by seeing an example at https://github.com/PlastecProfiles/EnrouteAddin
Back to Top
triangleMD View Drop Down
Expert
Expert


Joined: 14 March 2007
Location: USA
Points: 21
Post Options Post Options   Thanks (0) Thanks(0)   Quote triangleMD Quote  Post ReplyReply Direct Link To This Post Posted: 17 August 2016 at 7:28am
Can you also check the fact that the width option isn't accurate? For example, a routing offset with a 1/2" end mill with a width of cut set to .75" (2 steps) produces a toolpath with a width of .875". The width also grows with additional steps.
Back to Top
paloalto_17 View Drop Down
Admin Group
Admin Group


Joined: 29 October 2012
Location: United States
Points: 233
Post Options Post Options   Thanks (0) Thanks(0)   Quote paloalto_17 Quote  Post ReplyReply Direct Link To This Post Posted: 17 August 2016 at 1:29pm
The width of cut is functioning as intended, the problem is that when you apply a width of cut of .75 inches that does not mean that your cut is only going to be .75 inches wide. The width of cut is usually defined with a clean cut but can be cut with the rough pass. The width of cut refers to the amount of material that is left over for the clean pass to cut. Or if you only have a rough tool with 2 passes on the width set then it splits the .75 in half and it cuts .375 inches away from the material on the first pass then exactly on the part on the second pass. When it does this it does not mean its going to be constrained to only .75 in total width. I have created a video here that maybe helps with understanding the width of cut when only using it with a Rough tool. 

http://screencast.com/t/h7nOsG0NYJO

Best regards,
Aaron
Back to Top
 Post Reply Post Reply Page  12>
  Share Topic   

Forum Jump Forum Permissions View Drop Down

Forum Software by Web Wiz Forums® version 11.03
Copyright ©2001-2015 Web Wiz Ltd.